Help Center

3D Module

Options 3D Tab

The tab is used to configure 3D settings 3D. The tab is available with a license for 3D.

      ·    Common settings

      ·    2D views

      ·    Pseudo section properties

Common settings

CAD drafting 3D Module 0

Automatically project edges on sketch

The parameter when adding a new sketch adjusts the display of the projection of the edges of a flat face taken as the working plane for the sketch.

Call command "Add planar sketch".

CAD software 3D Module 1

Specify a flat face as a work plane.

CAD drawing 3D Module 2

Depending on the setting, a projection will be added to the sketch.

Yes

No

CAD drafting 3D Module 3

CAD software 3D Module 4

Automatically project the origin point on new sketch

Controls the projection of the origin point when creating a new sketch.

Yes

No

CAD drawing 3D Module 5

CAD drafting 3D Module 6

Automatically correct UCS while editing block references with 2D constraints

Automatic correction of UCS when editing a block reference with 2D constraints.

Restory viewport's camera while exiting 2D sketch editing mode

If enabled, the view camera will be in position before the sketch is edited.

Edit parametric constraint value upon creation

Controls whether the dependency editing dialog is opened immediately after installation.

CAD software 3D Module 7

Associativity for new bodies

The enabled option allows you to build fixed bodies without the possibility of defixation. The sketch must be attached to some plane.

Layer for sketches

It allows you to customize the name of the layer on which will be placed flat sketches.

Layer for working objects

It allows you to customize the name of the layer on which the objects will be located.

Layer for sections

It allows you to customize the name of the layer on which section will be located.

Layer for parametric 3D solids

Allows you to set the name of the layer on which the parametric 3D bodies will be located.

Show/no thread helix

Controls the display of the thread helix.

Thread helix color

Thread helix color.

Thread face color

Thread face color.

Mass display accuracy

Mass display accuracy for inspector properties and part and assembly unit properties.

2D views

CAD drawing 3D Module 8

Automatic update

Sets the update mode 2D views

Layer

It defines the layer which will be located 2D views

Visible lines

Show on sections

Adjusts the image visible lines on sections

Line color

Specifies the color of visible lines

Linetype

Specify the type of visible lines

Lineweight

It determines the weight of visible lines

Hidden lines

Show on sections

It adjusts the display of invisible lines on 2D views

Line color

Specifies the color of hidden lines

Linetype

Specify the type of hidden lines

Lineweight

It determines the weight of invisible lines

Section border

Settings differ from visible

It determines whether the parameters are different boundary lines of the section visible lines

If not, the next line settings are not valid.

Line color

Specifies the color of the boundary line section

Linetype

Specifies the type of the boundary line section

Lineweight

It determines the weight of the boundary line section

Hatch

Show

It controls the display of hatching

Face hatch

Settings such as shading

 3D. Pseudo section properties

CAD drafting 3D Module 9

Hatch

Show

It controls the display of hatching.

Face hatch

Settings such as shading.

Surface transparency

Settings such as shading. Default 0 - full transparency.

3D History

CAD software 3D Module 10Main menu: 3D - CAD drawing 3D Module 113D History...

CAD drafting 3D Module 12Ribbon: 3D Tools - Modeling - CAD software 3D Module 133D History.

CAD drawing 3D Module 14Functional panel: 3D History.

CAD drafting 3D Module 15Command line: SHOWTAB3DHISTORYNET.

CAD software 3D Module 16Command line: TABS - select "3D History".

When working in the 3D-design environment, a functional panel containing the model building tree is displayed on the screen. 

Building tree - sequence of objects (actions) that make up the model. 

CAD drawing 3D Module 17

Interface

The build tree contains a set of tools:

CAD drafting 3D Module 18Filter Items - massively hides all working objects: planes, axes, points.

CAD software 3D Module 19Update tree - updates the tree.

CAD drawing 3D Module 20Expand parts - expands all branches in the tree.

CAD drafting 3D Module 21Expand parts with errors - expands branches of parts that have errors.

CAD software 3D Module 22Collapse parts - collapses all expanded branches in the tree.

CAD drawing 3D Module 23Update model with regen(3drebuild) - rebuild model.

CAD drafting 3D Module 24Update model(mchist3dupdate) - update model.

CAD software 3D Module 25Assembly properties - opens the "Properties of an assembly unit" dialog, where the data of the selected object for the specification is specified.

Objects of a tree

CAD drawing 3D Module 26 - root folder "GCS" (General Coordinate System).

The following objects are bound to it:

     ·     CAD drafting 3D Module 27 - planes YZ, ZX, XY. By default, they are hidden and have a gray icon  CAD software 3D Module 28.

The following shortcut menu commands are available:

                 ·     Hide - hides the mapping of the plane in model space.

                 ·     Show - shows the mapping of the plane in model space.

                 ·     ShowInDocument - focuses the plane in the center of the model space. The command is available when the plane is displayed.

                 ·     Create 2d-sketch - call command "Add planar sketch". Sketch drawing plane is not necessary.

     ·     CAD drawing 3D Module 29 - axis oX, oY, oZ. By default, they are hidden and have a gray icon  CAD drafting 3D Module 30.

The following shortcut menu commands are available:

                 ·     Hide - the command hides the display of the axis in model space.

                 ·     Show - the command displays the axis in model space.

                 ·     ShowInDocument - the team focuses the axis in the center of the model space. The command is available when the axis is displayed.

     ·     CAD software 3D Module 31 - origin. Default is hidden and has a gray icon  CAD drawing 3D Module 32.

The following shortcut menu commands are available:

                 ·     Hide - the command hides the display of the origin in the model space.

                 ·     Show - the command shows the display of the origin in the model space.

                 ·     ShowInDocument - the team focuses the origin in the center of the model space. The command is available when the origin is displayed.

CAD drafting 3D Module 33 - root folder "Sections".

The following objects are bound to it:

     ·      CAD software 3D Module 34 - Section. Has child objects CAD drawing 3D Module 35View, taken from section.

CAD drafting 3D Module 36 - Planar sketch. When applied to it, 3D Operations is bound to an operation (becomes its child element) and the icon becomes inactive. An exception - assembly sketch.

CAD software 3D Module 37 - Part. It is a 3D object. Sheet bodies have their own icon  CAD drawing 3D Module 38.

The following objects can be attached to the part:

     ·     CAD drafting 3D Module 39"Planar sketch".

     ·     CAD software 3D Module 40"Work plane". Can be located in the root of the tree and enter the structure of objects CAD drawing 3D Module 41"Part".

     ·     CAD drafting 3D Module 42"Work axis". Can be located in the root of the tree and enter the structure of objects CAD software 3D Module 43"Part".

     ·     CAD drawing 3D Module 44"Work point". Can be located in the root of the tree and enter the structure of objects CAD drafting 3D Module 45"Part".

     ·     CAD software 3D Module 46"McExtrudeFeature". 3D operation.

     ·     CAD drawing 3D Module 47"McRevolveFeature". 3D operation.

     ·     CAD drafting 3D Module 48"McSweepFeature". 3D operation.

     ·     CAD software 3D Module 49"McLoftFeature". 3D operation.

     ·     CAD drawing 3D Module 50"Union". Contains the union parts.

     ·     CAD drafting 3D Module 51"Intersect". Contains the intersect parts.

     ·     CAD software 3D Module 52"Subtract". Contains the substract parts.

     ·     CAD drawing 3D Module 53"McChamferFeature".

     ·     CAD drafting 3D Module 54"McFilletFeature".

     ·     CAD software 3D Module 55"McMirrowFeature".

     ·     CAD drawing 3D Module 56"McRectangularPatternFeature".

     ·     CAD drafting 3D Module 57"McCircularPatternFeature".

     ·     CAD software 3D Module 58CAD drawing 3D Module 59CAD drafting 3D Module 60CAD software 3D Module 61CAD drawing 3D Module 62 - 3D constraints.

     ·     CAD drafting 3D Module 63 Nonparametric solid.

     ·     CAD software 3D Module 64End of builds. The object indicates the end of the body construction.

The following shortcut menu commands are available for the object CAD drawing 3D Module 65"Part":

     ·     Rename (F2) - allows you to rename the part.

     ·     Delete (Del) - removes the part and child objects from the tree and model space.

     ·     Hide - hides the part and child objects from the model space.

     ·     Show - shows the part and child objects in the model space.

     ·     Fix - fixes the part in space. You can not move (3D Move), rotate (3D Rotate) or align (3D Align). The part acquires an icon with an anchor CAD drafting 3D Module 66.

     ·     Unfix - de-fixes the part. You can move (3D Move), rotate (3D Rotate) or align (3D Align).

     ·     ShowInDocument - focuses and highlights the part in the center of the model space.

     ·     Rebuild - rebuilds an object in model space.

     ·     Create detail - creates a detailCAD software 3D Module 67from the part, internal objects are hidden. The detail is a 3d block.

CAD drawing 3D Module 68 Detail - the object is a 3D block.

The following shortcut menu commands are available for the object CAD drafting 3D Module 69 "Detail":

     ·     Open in editor - opens the 3D block editor.

     ·     Edit in place - opens the 3D reference editor.

     ·     Rename (F2) - allows you to rename the detail.

     ·     Delete (Del) - removes the detail and child objects from the tree and model space.

     ·     Hide - hides the detail and child objects from the model space.

     ·     Show - shows the detail and child objects in the model space.

     ·     Fix - fixes the detail in space. You can not move (3D Move), rotate (3D Rotate) or align (3D Align). The detail acquires an icon with an anchor CAD software 3D Module 70.

     ·     Unfix - de-fixes the detail. You can move (3D Move), rotate (3D Rotate) or align (3D Align).

     ·     ShowInDocument - focuses and highlights the detail in the center of the model space.

     ·     Rebuild - rebuilds an object in model space.

     ·     Disband - breaks a detail (assembly) into its component parts.

     ·     Create assembly - the command is active when two or more parts (details, assemblies) are selected and creates an assembly unit CAD drawing 3D Module 71 . The assembly is a 3d block.

     ·     Properties - command opens the "Properties" dialog.

CAD drafting 3D Module 72Assembly - an object is a 3d block that includes several units of parts, bodies, assemblies. Context menu commands are similar to the object  CAD software 3D Module 73 "Detail":

Modeling modes

CAD drawing 3D Module 74

Various types of modeling are used in the design process: Parametric, Direct, Sheet, Meshes.

Placing all of the commands for these types of modeling on the same tab at the same time creates confusion.

For the convenience of designing, the "Modeling modes" ribbon block has been added, which includes the following commands:

CAD drafting 3D Module 75Ribbon: 3D Tools - Modeling modes - CAD software 3D Module 76Parametric.

CAD drawing 3D Module 77Command line: 3DDRAFTINGMODE0.

Opens ribbon blocks "Parametric Modeling", "2D Sketch".

CAD drafting 3D Module 78

CAD software 3D Module 79Ribbon: 3D Tools - Modeling modes - CAD drawing 3D Module 80Direct.

CAD drafting 3D Module 81Command line: 3DDRAFTINGMODE1.

Opens ribbon block "Direct Modeling".

CAD software 3D Module 82

CAD drawing 3D Module 83Ribbon: 3D Tools - Modeling modes - CAD drafting 3D Module 84Sheet.

CAD software 3D Module 85Command line: 3DDRAFTINGMODE2.

Opens ribbon blocks "Sheet solids", "2D Sketch".

CAD drawing 3D Module 86

CAD drafting 3D Module 87Ribbon: 3D Tools - Modeling modes - CAD software 3D Module 88Meshes.

CAD drawing 3D Module 89Command line: 3DDRAFTINGMODE3.

Opens ribbon block "Mesh".

CAD drafting 3D Module 90

Sketch mode

Add planar sketch

CAD software 3D Module 91Main menu: 3D - 2D Sketch - CAD drawing 3D Module 92Add planar sketch.

CAD drafting 3D Module 93Ribbon: 3D Tools - 2D Sketch - CAD software 3D Module 94Add sketch.

CAD drawing 3D Module 95Toolbar: 3D - CAD drafting 3D Module 96Add planar sketch.

CAD software 3D Module 97Command line: PSADD.

There are 2 ways to create a sketch, with a reference to the plane and without binding.

With a sketch without binding, a 3D operation is created in the new unfixed body.

From the sketch with reference to the plane of the body, a 3D operation is created with a binding to the body.

From a sketch bound to a plane that does not belong to the body, a 3D operation is created in the new fixed body without the possibility of de-fixing.

Important!

When creating a sketch that will serve as a cross-section for 3D design operations, it is important to remember that the sketch must be a closed loop.

Creating a sketch without a reference to the plane

Sketching without reference to a plane is done in the XY plane.

1. Draw a sketch.

CAD drawing 3D Module 98

2. Select all sketch entities.

CAD drafting 3D Module 99

3. Call command CAD software 3D Module 100"Add planar sketch". The system automatically sets the desired view orientation. All the available objects in the sketch will be transferred from the selected objects.

CAD drawing 3D Module 101

4. Finish sketch editing.

CAD drafting 3D Module 102

5. A sketch without reference to a plane will be created and added to  "3D History".

Creating a sketch with a reference to the plane

1. Call command CAD software 3D Module 103"Add planar sketch".

2. Select the sketch creation plane. This can be a plane GCS, any working plane, as well as a flat surface of the body. The system automatically sets the desired orientation of the view - normal to the selected plane.

3. Draw a sketch.

CAD drawing 3D Module 104

For convenience, in sketch editing mode, the ribbon contains all the necessary commands to draw a sketch, edit its geometry, project some face, or complete sketch editing.

CAD drafting 3D Module 105

4. Finish sketch editing.

CAD software 3D Module 106

5. A sketch with a reference to the plane will be created and added to  "3D History".

Properties

Does not have individual properties.

Grips

CAD drawing 3D Module 107Moving grip - is used to move the sketch in model space.

3D History

CAD drafting 3D Module 108 "Planar sketch". When creating Planar sketch is located in the root of the tree. When applied to it, 3D Operations is bound to an operation (becomes its child element) and the icon becomes inactive. An exception - Assembly sketch.

he following shortcut menu commands are available:

     ·     Edit - Calls to edit the sketch. To the right of the icon appears the editing symbol CAD software 3D Module 109.

     ·     End edit - completes the previously started editing.

     ·     Rename (F2) - allows you to rename a sketch.

     ·     Delete (Del) - removes a sketch from the tree and model space.

     ·     Hide - hides a sketch from the model space. The icon becomes inactive.

     ·     Show - shows a sketch in model space. The icon becomes active.

     ·     Suppress - removes the thumbnail from the model space. The icon becomes inactive. Suppressed elements are removed only from the model space, while they remain in the build tree. After suppressing the element, the model will be rebuilt without taking into account the excluded elements and their derivatives.

     ·     Unsuppress - restores a sketch in model space. 

     ·     ShowInDocument - focuses and highlights the sketch in the center of the model space.

     ·     Rebuild - rebuilds the object in model space.

Add assembly sketch

CAD drawing 3D Module 110Main menu: 3D - 2D Sketch - CAD drafting 3D Module 111Add assembly sketch.

CAD software 3D Module 112Toolbar: 3D - CAD drawing 3D Module 113Add assembly sketch.

CAD drafting 3D Module 114Command line: PSADDASM.

The command is similar  "Add planar sketch".

Differences of the assembly sketch

     ·     the assembly sketch is not included in any body, including in the model tree;

     ·     the body constructed from the assembly sketch is automatically fixed in the last position without the possibility of a defect;

     ·     the body built from the assembly sketch can only be moved together with the assembly sketch. You can only move the sketch.

Include object to sketch

CAD software 3D Module 115Main menu: 3D - 2D Sketch - CAD drawing 3D Module 116Include object to sketch.

CAD drafting 3D Module 117Ribbon: 3D Tools - 2D Sketch - CAD software 3D Module 118Include Object.

CAD drawing 3D Module 119Toolbar: 3D - CAD drafting 3D Module 120Include object to sketch.

CAD software 3D Module 121Command line: PSINCL.

The command is used to add objects not built in sketch mode to the sketch. The command is available in the mode of creating (editing) the sketch.

Procedure

1. In sketch editing mode, call the command CAD drawing 3D Module 122"Include object to sketch".

CAD drafting 3D Module 123

2. Specify the objects that you want to add to the sketch. The object is added to the sketch.

CAD software 3D Module 124

3. To exit the add mode, press  "Esc".

Add projection to sketch

CAD drawing 3D Module 125Main menu: 3D - 2D Sketch - CAD drafting 3D Module 126Add projection to sketch.

CAD software 3D Module 127Ribbon: 3D Tools - 2D Sketch - CAD drawing 3D Module 128Add Projection.

CAD drafting 3D Module 129Toolbar: 3D - CAD software 3D Module 130Add projection to sketch.

CAD drawing 3D Module 131Command line: PSPROJ.

The team projects geometry that is not built in sketch mode. It is also possible to project the geometry from the bodies. The command is available in the mode of creating (editing) the sketch.

Procedure

1. In sketch editing mode, call the command CAD drafting 3D Module 132"Add projection to sketch".

CAD software 3D Module 133

2. Sequentially indicate the edges of the object that you want to project. The projection is performed automatically immediately after the indication.

CAD drawing 3D Module 134

3. To exit the loop, press  "Esc".

Important!

When you remove the projected geometry, the projection is removed along with the geometry.

Features of work

Projected geometry in a sketch can be redefined to another of that type. In this case, all associative bindings are preserved.

To override you need:

1. Call the sketch for editing;

CAD drafting 3D Module 135

2. Select the projected geometry;

CAD software 3D Module 136

3. Call the RMB context menu and select the "Redefine" command;

4. Specify another edge of the object, it must have the same type (line, circle...);

CAD drawing 3D Module 137

5. The geometry will be redefined. Associative links will be preserved.

CAD drafting 3D Module 138

Redefine plane for sketch

CAD software 3D Module 139Main menu: 3D - 2D Sketch - CAD drawing 3D Module 140Redefine plane for sketch.

CAD drafting 3D Module 141Ribbon: 3D Tools - 2D Sketch - CAD software 3D Module 142Redefine Plane.

CAD drawing 3D Module 143Toolbar: 3D - CAD drafting 3D Module 144Redefine plane for sketch.

CAD software 3D Module 145Command line: PSREDEFINE.

The command changes the plane of the selected sketch to another flat surface or work plane.

Procedure

1. Call command CAD drawing 3D Module 146"Redefine plane for sketch".

2. Select in the model space or in the "3D History" sketch to move.

CAD drafting 3D Module 147

3. Select a new plane for the sketch in model space, in "3D History" or GCS plane from the context menu.

CAD software 3D Module 148

4. The sketch will be automatically moved to another plane.

Set Sketch Coordinate System

CAD drawing 3D Module 149Main menu:  3D - 2D Sketch - CAD drafting 3D Module 150Set Sketch Coordinate System.

CAD software 3D Module 151Ribbon: 3D Tools - 2D Sketch - CAD drawing 3D Module 152Set Sketch Coordinate System.

CAD drafting 3D Module 153Toolbar: 3D - CAD software 3D Module 154Set Sketch Coordinate System.

CAD drawing 3D Module 155Command line: PSDEFINECS.

When you sketch on a planar face or work plane, the system automatically creates the sketch coordinate system. The "Set Sketch Coordinate System" command is required to edit the coordinate system of the selected sketch.

Procedure

1. A sketch must first be created on a work plane or planar face.

CAD drafting 3D Module 156

2. Call command CAD software 3D Module 157"Set Sketch Coordinate System" and specify a flat sketch if necessary.

3. The sketch coordinate system is displayed.

CAD drawing 3D Module 158

4. Select the item to change. The X, Y axis, or the origin point can be used as the element to change.

Point

Axis

CAD drafting 3D Module 159

CAD software 3D Module 160

5. Pick a new position for the element. To change the origin, you need to specify a new point; to change the direction of the axis, you need to specify any straight edge. The position of the sketch relative to its coordinate system does not change.

Point

Axis

CAD drawing 3D Module 161

CAD drafting 3D Module 162

6. The sketch coordinate system will be changed.

Edit planar sketch

CAD software 3D Module 163Main menu: 3D - 2D Sketch - CAD drawing 3D Module 164Edit planar sketch.

CAD drafting 3D Module 165Ribbon: 3D Tools - 2D Sketch - CAD software 3D Module 166Edit sketch.

CAD drawing 3D Module 167Toolbar: 3D - CAD drafting 3D Module 168Edit planar sketch.

CAD software 3D Module 169Command line: PSEDIT.

CAD drawing 3D Module 170Context menu: Command "Edit" on select sketch in "3D History".

The command switches to edit mode a flat sketch.

Procedure

1. Specify in the model space or in the "3D History" sketch.

2. Call command CAD drafting 3D Module 171"Edit planar sketch".

3. The sketch will go into edit mode.

End editing

CAD software 3D Module 172Main menu: 3D - 2D Sketch - CAD drawing 3D Module 173End editing.

CAD drafting 3D Module 174Ribbon: 3D Tools - 2D Sketch - CAD software 3D Module 175End editing.

CAD drawing 3D Module 176Toolbar: 3D - CAD drafting 3D Module 177End editing.

CAD software 3D Module 178Command line: PSENDEDIT.

The command finishes creating or editing a sketch.

Parametric modeling

3D Extrude

CAD drawing 3D Module 179Main menu: 3D - 3D Features - CAD drafting 3D Module 1803D Extrude.

CAD software 3D Module 181Ribbon: 3D Tools - Modeling - CAD drawing 3D Module 1823D Extrude.

CAD drafting 3D Module 183Toolbar: 3D - CAD software 3D Module 1843D Extrude.

CAD drawing 3D Module 185Command line: 3DEXTRUDE.

Tool for pulling a section along a straight path.

Procedure

1. Create a Planar sketch (if it is not).

2. Call command CAD drafting 3D Module 186"3D Extrude". Open dialog "3D Extrude".

CAD software 3D Module 187

3. Specify the required options in the dialog box "3D Extrude":

     ·     Select the section sketch. Possible sketches are highlighted by horizontal hatching. The selected section is highlighted by vertical shading. The sketch must be a closed loop.

Note:

If you have already selected a section from one sketch, and you want to select another section from another sketch, you must first deselect the section you have already selected.

CAD drawing 3D Module 188

Simultaneously with the selection of the section, a contour of the extruded section appears - a preview of the result of the operation.

CAD drafting 3D Module 189

     ·     Set the extrusion distance.

     ·     Choose a direction: Positive, Negative, Both directions.

     ·     Specify, if necessary, the slope of the extrusion.

4. Press button "OK". The operation will be carried out. If the "OK" button is not active, then the sketch was not selected or the parameters were incorrectly set. In the "3D History" will be created object CAD software 3D Module 190"McExtrudeFeature", containing a sketch, linked to an existing or a new body.

 

Dialog

Button CAD drawing 3D Module 191"Profile" - allows you to select in the model space or in the "3D History" sketch.

Button CAD drafting 3D Module 192"TgSolid" - allows you to specify the parent body for the sketch.

Switch "New body is associative" - controls the settings parameter "Associativity when creating new bodies". The enabled

 option allows you to build fixed bodies without the possibility of defixation.

A group of operation action selectors:

     ·     CAD software 3D Module 193"Join" - creates a new extrusion object in the previously created body. The sketch must belong to the body.

     ·     CAD drawing 3D Module 194"Cut" - creates a cutout with the outline of the selected sketch (for example, holes). When cutting, the dimension selection field becomes active, allowing you to select the cut length to a distance or through. The sketch must belong to the body.

     ·     CAD drafting 3D Module 195"Intersect" - creates an object to intersect the contours of the new sketch and the previously created body. The sketch must belong to the body.

     ·     CAD software 3D Module 196"New body" - creates a new extrusion object. A new body appears in the tree of constructions. When a switch is selected, the previously selected sketch belonging to the body is detached from the body.

Extends:

     ·     CAD drawing 3D Module 197"The field for selecting the type of dimension". Distance - extrusion, cutting or intersection is specified by the distance. All - cutting is carried out through the whole body, the distance input field is unavailable.

     ·     Field CAD drafting 3D Module 198"Distance" - allows you to specify the distance. To the right of the field, there is a button to indicate the distance from the drawing.

     ·     CAD software 3D Module 199"Group of direction selection switches" - controls the direction of extrusion relative to the sketch plane.

CAD drawing 3D Module 200Positive direction - directs the extrusion towards the positive direction of the axis perpendicular to the plane of the sketch.

CAD drafting 3D Module 201Negative direction -directs the extrusion towards the negative direction of the axis perpendicular to the plane of the sketch.

CAD software 3D Module 202Both direction - directs extrusion in both directions relative to the sketch plane by the same distance.

FieldCAD drawing 3D Module 203"Angle of slope" - allows you to specify the angle of inclination. The operation creates a body tapering to a point. To the right of the field there is a button for specifying the angle from the drawing.

Note:

When choosing the faces of an existing body for building 3D-operations, it is recommended to disable the Center binding in order to avoid incorrect work.

Select new body

There are two bodies: a cylinder and a parallelepiped. On the upper plane of the cylinder a sketch is created, which is a circle whose center is located between these bodies.

CAD drafting 3D Module 204

Call the "3D Extrude" dialog and select this circle as the sketch. As an action, select "Cut". By default, the sketch belongs to the body on whose plane it was built, in this case the cylinder. Correspondingly, the cutting will be performed for the cylinder.

CAD software 3D Module 205

By default, the body of the cylinder is selected.

CAD drawing 3D Module 206

Assign a new body to the parallelepiped, for which we click on the button CAD drafting 3D Module 207"TgSolid" and the LMC we select a parallelepiped.

CAD software 3D Module 208

Result: the sketch belongs to the body of Parallelepiped, is part of its tree, and makes a cutout in its body.

CAD drawing 3D Module 209

 

3D History

CAD drafting 3D Module 210"McExtrudeFeature". It is part of the body.

The following shortcut menu commands are available:

     ·     Edit - calls for editing a 3D operation. To the right of the icon appears the editing symbol CAD software 3D Module 211.

     ·     End edit - completes the previously started editing.

     ·     Rename (F2) - allows you to rename a 3D operation.

     ·     Delete (Del) - removes the 3D operation and child objects from the tree and model space.

     ·     Suppress - removes the 3D operation and child objects from the model space.

     ·     Unsuppress - restores a 3D operation in model space.

     ·     ShowInDocument - focuses and highlights the 3D operation in the center of the model space.

     ·     Rebuild - rebuilds the object in model space.

3D Revolve

CAD drawing 3D Module 212Main menu: 3D - 3D Features - CAD drafting 3D Module 2133D Revolve.

CAD software 3D Module 214Ribbon: 3D Tools - Modeling - CAD drawing 3D Module 2153D Revolve.

CAD drafting 3D Module 216Toolbar: 3D - CAD software 3D Module 2173D Revolve.

CAD drawing 3D Module 218Command line: 3DREVOLVE.

Tool for drawing a section along a path in the form of a circle or a circular segment.

Procedure

1. Create a Planar sketch (if it is not).

2. Create a working axis, if necessary, around which the rotation will take place. The face of the body can also serve as an axis.

3. Call command CAD drafting 3D Module 219"3D Revolve". Open dialog "3D Revolve".

CAD software 3D Module 220

4. Specify the required options in the dialog box  "3D Revolve":

     ·     Select the section sketch. Possible sketches are highlighted by horizontal hatching. The selected section is highlighted by vertical shading. The sketch must be a closed loop.

Note:

If you have already selected a section from one sketch, and you want to select another section from another sketch, you must first deselect the section you have already selected.

CAD drawing 3D Module 221

     ·     Select the axis of rotation. You can select the line in the drawing, including the line that is part of the sketch, as well as the edge of the body. A preview of the results of the operation appears.

 

     ·     Set the rotation angle and direction if necessary.

CAD drafting 3D Module 222

5. Press button "OK". The operation will be carried out. If the "OK" button is not active, then the sketch, axis, or incorrect parameters were not selected. In the "3D History" will be created object CAD software 3D Module 223"McRevolveFeature", a sketch containing a sketch, linked to an existing or a new body.

Note:

When choosing the faces of an existing body for building 3D-operations, it is recommended to disable the Center binding in order to avoid incorrect work.

Dialog

Button CAD drawing 3D Module 224"Profile" - allows you to select in the model space or in the "3D History" sketch.

Button CAD drafting 3D Module 225"Axis" - allows you to select the axis of rotation in the model space or in the "3D History".

Button CAD software 3D Module 226"TgSolid" - allows you to specify the parent body for the sketch (for more information about the function, see Extrude).

Switch "New body is associative" - controls the settings parameter "Associativity when creating new bodies". The enabled option allows you to build fixed bodies without the possibility of defixation.

A group of operation action selectors:

     ·     CAD drawing 3D Module 227"Join" - creates a new object by rotating in the previously created body. The sketch must belong to the body.

     ·     CAD drafting 3D Module 228"Cut" - creates a cutout by rotating the selected sketch (for example, holes). The sketch must belong to the body.

     ·     CAD software 3D Module 229"Intersect" - creates an object to intersect the contours of the new sketch and the previously created body. The sketch must belong to the body.

     ·     CAD drawing 3D Module 230"New body" - creates a new rotation object. A new body appears in the tree of constructions. When a switch is selected, the previously selected sketch belonging to the body is detached from the body.

Extents:

     ·     CAD drafting 3D Module 231"The field for selecting the type of dimension". RevAngle - rotation is given by the angle. FullRev - rotation is performed on a full circle.

     ·     Field CAD software 3D Module 232"Angle" - allows you to specify the rotation angle. To the right of the field there is a button for specifying the angle from the drawing.

     ·     CAD drawing 3D Module 233"Group of direction selection switches" - controls the direction of extrusion relative to the sketch plane.

CAD drafting 3D Module 234Positive direction - directs the rotation toward the positive direction of the axis perpendicular to the plane of the sketch. 

CAD software 3D Module 235Negative direction - directs the rotation toward the negative direction of the axis perpendicular to the plane of the sketch.

CAD drawing 3D Module 236Both direction - directs the rotation in both directions relative to the sketch plane by the same distance.

3D History

CAD drafting 3D Module 237"McRevolveFeature". It is part of the body.

The following shortcut menu commands are available:

     ·     Edit - calls for editing a 3D operation. To the right of the icon appears the editing symbol CAD software 3D Module 238.

     ·     End edit - completes the previously started editing.

     ·     Rename (F2) - allows you to rename a 3D operation.

     ·     Delete (Del) - removes the 3D operation and child objects from the tree and model space.

     ·     Suppress - removes the 3D operation and child objects from the model space. 

     ·     Unsuppress - restores a 3D operation in model space.

     ·     ShowInDocument - focuses and highlights the 3D operation in the center of the model space.

     ·     Rebuild - rebuilds the object in model space.

3D Sweep

CAD drawing 3D Module 239Main menu: 3D - 3D Features - CAD drafting 3D Module 2403D Sweep.

CAD software 3D Module 241Ribbon: 3D Tools - Modeling - CAD drawing 3D Module 2423D Sweep.

CAD drafting 3D Module 243Toolbar: 3D - CAD software 3D Module 2443D Sweep.

CAD drawing 3D Module 245Command line: 3DSWEEP.

Tool for drawing a section along a previously trajectory.

Procedure

1. Create a Planar sketch (if not).

2. Create a path along which the section will be drawn. The trajectory must be drawn in another sketch mode in the orthogonal plane to the section plane.

3. Call command CAD drafting 3D Module 246"3D Sweep". Open dialog "3D Sweep".

CAD software 3D Module 247

4. Specify the required options in the dialog box "3D Sweep":

     ·     Select the section sketch. Possible sketches are highlighted with purple fill. The sketch must be a closed loop.

Note:

If you have already selected a section from one sketch, and you want to select another section from another sketch, you must first deselect the section you have already selected.

The selected section is highlighted with a green fill.

CAD drawing 3D Module 248CAD drafting 3D Module 249

     ·     Select a path. If the path is a polyline or a combination of individual lines, you must select a path in sequence. To exclude from the sequence an incorrectly selected path segment, you must click on it LMC + Shift.

CAD software 3D Module 250CAD drawing 3D Module 251

     ·     Select an orientation.

Along path

Parallel

CAD drafting 3D Module 252

CAD software 3D Module 253

     ·     If necessary, specify the broadening (if the orientation is selected along the path).

5. Press button "OK". The operation will be carried out. If the "OK" button is not active, then the sketch, the trajectory was not selected, or the parameters were incorrectly set. In the "3D History" will be create object CAD drawing 3D Module 254"McSweepFeature", containing a sketch and trajectory, with reference to an existing or a new body.

Note:

When choosing the faces of an existing body for building 3D-operations, it is recommended to disable the Center binding in order to avoid incorrect work.

Dialog

Button CAD drafting 3D Module 255"Profile" - allows you to select in the model space or in the "3D History" sketch.

Button CAD software 3D Module 256"Path" - allows you to select a trajectory in the model space or in the "3D History".

Button CAD drawing 3D Module 257"TgSolid" - allows you to specify the parent body for the sketch (For more information about the function, see Extrude).

Switch "New body is associative" - controls the settings parameter "Associativity when creating new bodies". The enabled option allows you to build fixed bodies without the possibility of defixation.

A group of operation action selectors:

     ·     CAD drafting 3D Module 258"Join" - creates a new draw object in the previously created body. The sketch must belong to the body.

     ·     CAD software 3D Module 259"Cut" - creates a cutout by drawing out the selected sketch (for example, holes). The sketch must belong to the body.

     ·     CAD drawing 3D Module 260"Intersect" - creates an object to intersect the contours of the new sketch and the previously created body. The sketch must belong to the body.

     ·     CAD drafting 3D Module 261"New body" - creates a new draw object. A new body appears in the tree of constructions. When a switch is selected, the previously selected sketch belonging to the body is detached from the body.

Parameters:

     ·     CAD software 3D Module 262"The field for selecting the type of dimension". Path - The pull length is given by the path. The field is not active.

     ·     Radiogroup "Orientation" - controls the orientation of the sketch sections: Along path - sections are drawn perpendicular to the path line; Parallel - sections are built parallel to the sketch.

CAD drawing 3D Module 263

     ·     Field CAD drafting 3D Module 264"Taper" - allows you to specify the angle of broadening. To the right of the field there is a button for specifying the angle from the drawing. The field is active when the track is oriented.

3D History

CAD software 3D Module 265"McSweepFeature". It is part of the body. Contains sketch and CAD drawing 3D Module 266"Path".

The following shortcut menu commands are available for the object  CAD drafting 3D Module 267"McSweepFeature":

     ·     Edit - calls for editing a 3D operation. To the right of the icon appears the editing symbol CAD software 3D Module 268.

     ·     End edit - completes the previously started editing.

     ·     Rename (F2) - allows you to rename a 3D operation.

     ·     Delete (Del) - removes the 3D operation and child objects from the tree and model space.

     ·     Suppress - removes the 3D operation and child objects from the model space. 

     ·     Unsuppress - restores a 3D operation in model space.

     ·     ShowInDocument - focuses and highlights the 3D operation in the center of the model space.

     ·     Rebuild - rebuilds an object in model space.

The following shortcut menu commands are available for the object  CAD drawing 3D Module 269"Path":

     ·     Edit - causes editing of the trajectory.

     ·     End edit - completes the previously started editing.

     ·     Hide - hides the trajectory from the model space.

     ·     Show - shows the trajectory in the model space.

     ·     ShowInDocument - focuses and highlights the trajectory in the center of the model space.

     ·     Rebuild - rebuilds an object in model space.

3D Loft

CAD drafting 3D Module 270Main menu: 3D - 3D Features - CAD software 3D Module 2713D Loft.

CAD drawing 3D Module 272Ribbon: 3D Tools - Modeling - CAD drafting 3D Module 2733D Loft.

CAD software 3D Module 274Toolbar: 3D - CAD drawing 3D Module 2753D Loft.

CAD drafting 3D Module 276Command line: 3DLOFT.

Tool for drawing bodies with different sections.

Procedure

1. Create Planar sketches with sections.

2. Call command CAD software 3D Module 277"3D Loft". Open dialog "3D Loft".

CAD drawing 3D Module 278

3. Specify the required options in the dialog box  "3D Loft":

     ·     Select the first section. The sketch of a section must be a closed contour. The first section in the list can not be deleted. By clicking the "Delete" button, the geometry set for this section is cleared. After that, the geometry can be selected again. In the dialog, changing the color of the arrow means that the contour of the section is selected and you can proceed to select the next forming section.

     ·     Add the following sections. To add a section, click the "Add" button. When adding sections, the preliminary result of the operation will be shown. The number of forming sections is not limited.

CAD drafting 3D Module 279CAD software 3D Module 280

Note:

You can not add a new section without completing the geometry selection for the previous section.

 

Note:

If you have already selected a section from one sketch, and you want to select another section from another sketch, you must first deselect the section you have already selected.

     ·     Select the type of rails: Rails or Center line. For more information on rails, see below.

     ·     If necessary, specify Rails or Center line. For more information on guides, see below.

4. Press button "OK". The operation will be performed.

CAD drawing 3D Module 281

Dialog

Switch "New body is associative" - controls the settings parameter "Associativity when creating new bodies". The enabled option allows you to build fixed bodies without the possibility of defixation.

A group of operation action selectors:

     ·     CAD drafting 3D Module 282"Join" - creates a new object in the previously created body. The sketch must belong to the body.

     ·     CAD software 3D Module 283"Cut" - creates a cutout. The sketch must belong to the body.

     ·     CAD drawing 3D Module 284"Intersect" - creates an object to intersect the contours of the new sketch and the previously created body. The sketch must belong to the body.

     ·     CAD drafting 3D Module 285"New body" - creates a new object. A new body appears in the tree of constructions. When a switch is selected, the previously selected sketch belonging to the body is detached from the body.

Ribbon Selection Panel:

     ·     CAD software 3D Module 286 Rails 

     ·     CAD drawing 3D Module 287Center line

List of sections. Contains a list of selected sections

CAD drafting 3D Module 288

List of rails. Contains a list of selected curve rails.

CAD software 3D Module 289

Rails

Rails determine the form of stretching across sections between sections.

Rails can be 2D or 3D curves or edges of an existing body. The number of rails is unlimited. Rails affect the whole form of stretching across sections, not just vertices.

Rails must pass strictly through each contour of drawing by sections. In this case, the start of the rail must be strictly on the contour of the first section, the end of the rail strictly on the contour of the last section.

Rail must not be interrupted.

It is possible to construct closed rails - in this case a closed body will be constructed.

The following guide curves are not allowed:

CAD drawing 3D Module 290

Example of using rails:

Without the use of rails

Using rails

CAD drafting 3D Module 291

CAD software 3D Module 292

CAD drawing 3D Module 293

CAD drafting 3D Module 294

 

Note:

Rail curves do not work when the "Close" option is selected.

Center line

The centerline is the type of the railing curve. The center line must pass through each section. The center line can be only one.

Without using a center line

Using a center line

CAD software 3D Module 295

CAD drawing 3D Module 296

CAD drafting 3D Module 297

CAD software 3D Module 298

3D History

CAD drawing 3D Module 299"McLoftFeature". It is part of the body. Contains a list  CAD drafting 3D Module 300"Section".

The following shortcut menu commands are available for the object  CAD software 3D Module 301"McLoftFeature":

     ·     Edit - calls for editing a 3D operation. To the right of the icon appears the editing symbol CAD drawing 3D Module 302.

     ·     End edit - completes the previously started editing.

     ·     Rename (F2) - allows you to rename a 3D operation.

     ·     Delete (Del) - removes the 3D operation and child objects from the tree and model space.

     ·     Suppress - removes the 3D operation and child objects from the model space.

     ·     Unsuppress - restores a 3D operation in model space.

     ·     ShowInDocument - focuses and highlights the 3D operation in the center of the model space.

     ·     Rebuild - rebuilds the object in model space.

3D operation CAD drafting 3D Module 303"McLoftFeature" there are child objects  CAD software 3D Module 304"Section".

The following shortcut menu commands are available for the object  CAD drawing 3D Module 305"Section":

     ·     Delete (Del) - removes the section from the tree and model space.

Rebuild 3D model

CAD drafting 3D Module 306Main menu: 3D - CAD software 3D Module 307Rebuild 3D model.

CAD drawing 3D Module 308Ribbon: 3D Tools - Modeling - CAD drafting 3D Module 309Rebuild Model.

CAD software 3D Module 310Functional panel:3D History - CAD drawing 3D Module 311Rebuild 3D model.

CAD drafting 3D Module 312Command line: 3DREBUILD.

Tool for updating model parameters.

3D Solids

The section "3D Solids" describes the creation of dwg-compatible 3D solids. The resulting objects can be edited using standard AutoCAD tools.

Box

CAD software 3D Module 313Main menu: 3D - Solid - CAD drawing 3D Module 314Box.

CAD drafting 3D Module 315Ribbon: 3D Tools - 3D Solids - CAD software 3D Module 316Box.

CAD drawing 3D Module 317Toolbar: 3D Solid - CAD drafting 3D Module 318Box.

CAD software 3D Module 319Command line: 3DBOX.

The command create 3D solid - Box.

Procedure

1. Call command  CAD drawing 3D Module 320"Box".

2. Choose a point of reference (via context menu or command line): "Corner" (default) or "Center".

     ·     Corner - the sides of the box are counted from the specified point.

     ·     Center - the sides are counted evenly from the center.

3. Specify the starting point in the selected way.

4. Choose a base construction method: "Corner" (default), "Cube" or "Length".

     ·     Corner - a rectangle is constructed when specifying the second point.

     ·     Cube - the length, width and height will be the same and after specifying the point the box will be built.

     ·     Length - alternately indicate the length and width of the base.

5. Build the base in the chosen way.

CAD drafting 3D Module 321

6. Select the method of setting the height: "Height" (default) or "DistanceBy2Point".

     ·     Height - the height of the box is set in the drawing or in the command line.

     ·     DistanceBy2Point - the height of the box is specified by specifying two points in the drawing.

7. Specify the height of the selected method.

CAD software 3D Module 322

8. The box will be built.

CAD drawing 3D Module 323

Grips

1. Grips change the width and length of the base.

2. Grips change the width or length of the base.

3. Grips change the height of the box.

4. Grip moving object.

CAD drafting 3D Module 324

3D History

CAD software 3D Module 325"3D solid". It is part of the CAD drawing 3D Module 326body.

The following context menu commands are available:

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object and child objects from the tree and model space.

     ·     ShowInDocument - focuses and highlights the object in the center of the model space.

     ·     Rebuild - rearranges the object in the model space.

Cylinder

CAD drafting 3D Module 327Main menu: 3D - Solid - CAD software 3D Module 328Cylinder.

CAD drawing 3D Module 329Ribbon: 3D Tools - 3D Solids - CAD drafting 3D Module 330Cylinder.

CAD software 3D Module 331Toolbar: 3D Solid - CAD drawing 3D Module 332Cylinder.

CAD drafting 3D Module 333Command line: 3DCYLINDER.

The command create 3D solid - Cylinder.

Procedure

1. Call command  CAD software 3D Module 334"Cylinder".

2. Choose a base construction method:

     ·     Base center (default) - the circle is built in the center and radius.

     ·     3Point - the circle is built at three points.

     ·     RoundBaseBy2Point - build a circle at two points.

     ·     Incircle round base - a circle is constructed along two tangents.

     ·     Elliptical - an ellipse is built along the center, half-line and radius.

3. Specify the necessary parameters depending on the chosen method of building the foundation. The foundation will be built.

CAD drawing 3D Module 335

4. Choose a way to specify the height of the cylinder:

     ·     Height - indicates the height in the drawing or on the command line.

     ·     DistanceBy2Point - height is calculated by the specified two points in the drawing.

     ·     Axis endpoint - height and direction are calculated at the specified point in the drawing, the first reference point is the center of the base.

5. Specify the required parameters depending on the selected method of specifying the height.

CAD drafting 3D Module 336

6. The cylinder will be built.

CAD software 3D Module 337

Grips

1. Grips change the radius of the base.

2. Grips change the height of the cylinder.

3. Grip move.

CAD drawing 3D Module 338

3D History

CAD drafting 3D Module 339"3D solid". It is part of the CAD software 3D Module 340body.

The following context menu commands are available:

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object and child objects from the tree and model space.

     ·     ShowInDocument - focuses and highlights the object in the center of the model space.

     ·     Rebuild - rearranges the object in the model space.

Cone

CAD drawing 3D Module 341Main menu: 3D - Solid - CAD drafting 3D Module 342Cone.

CAD software 3D Module 343Ribbon: 3D Tools - 3D Solids - CAD drawing 3D Module 344Cone.

CAD drafting 3D Module 345Toolbar: 3D Solid - CAD software 3D Module 346Cone.

CAD drawing 3D Module 347Command line: 3DCONE.

The command create 3D solid - Cone.

Procedure

1. Call command  CAD drafting 3D Module 348"Cone".

2. Select the method for constructing the base: 

     ·     Base center (default) - the circle is built in the center and radius.

     ·     3Point - the circle is built at three points.

     ·     RoundBaseBy2Point - build a circle at two points.

     ·     Incircle round base - a circle is constructed along two tangents.

     ·     Elliptical - an ellipse is built along the center, half-line and radius.

3. Specify the necessary parameters depending on the chosen method of building the foundation. The foundation will be built.

CAD software 3D Module 349

4. Choose a way to specify the height of the cone:

     ·     Height - indicates the height in the drawing or on the command line.

     ·     DistanceBy2Point - height is calculated by the specified two points in the drawing.

     ·     Axis endpoint - height and direction are calculated at the specified point in the drawing, the first reference point is the center of the base.

     ·     Upper radius - first the radius of the upper base is indicated, then the height is indicated.

5. Specify the required parameters depending on the selected method of specifying the height.

CAD drawing 3D Module 350

6. The cone will be built.

CAD drafting 3D Module 351

Grips

1. Grips change the height of the cone.

2. Grip move.

3. Grip change the radius of the upper base.

4. Grips change the radius of the lower base.

CAD software 3D Module 352

3D History

CAD drawing 3D Module 353"3D solid". It is part of the CAD drafting 3D Module 354body.

The following context menu commands are available:

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object and child objects from the tree and model space.

     ·     ShowInDocument - focuses and highlights the object in the center of the model space.

     ·     Rebuild - rearranges the object in the model space.

Sphere

CAD software 3D Module 355Main menu: 3D - Solid - CAD drawing 3D Module 356Sphere.

CAD drafting 3D Module 357Ribbon: 3D Tools - 3D Solids - CAD software 3D Module 358Sphere.

CAD drawing 3D Module 359Toolbar: 3D Solid - CAD drafting 3D Module 360Sphere.

CAD software 3D Module 361Command line: 3DSPHERE.

The command create 3D solid - Sphere.

Procedure

1. Call command  CAD drawing 3D Module 362"Sphere".

2. Choose a way to build a sphere: 

     ·     Center (default) - the circle is built in the center and radius.

     ·     3Point - the circle is built at three points.

     ·     RoundBaseBy2Point - build a circle at two points.

     ·     Incircle round base - a circle is constructed along two tangents.

3. Specify the necessary parameters depending on the selected construction method.

CAD drafting 3D Module 363

4. Sphere will be built.

CAD software 3D Module 364

Grips

1. Grip move.

2. Grips change radius.

CAD drawing 3D Module 365

3D History

CAD drafting 3D Module 366"3D solid". It is part of the CAD software 3D Module 367body.

The following context menu commands are available:

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object and child objects from the tree and model space.

     ·     ShowInDocument - focuses and highlights the object in the center of the model space.

     ·     Rebuild - rearranges the object in the model space.

Pyramid

CAD drawing 3D Module 368Main menu: 3D - Solid - CAD drafting 3D Module 369Pyramid.

CAD software 3D Module 370Ribbon: 3D Tools - 3D Solids - CAD drawing 3D Module 371Pyramid.

CAD drafting 3D Module 372Toolbar: 3D Solid - CAD software 3D Module 373Pyramid.

CAD drawing 3D Module 374Command line: 3DPYRAMID.

The command create 3D solid - Pyramid.

Procedure

1. Call command  CAD drafting 3D Module 375"Pyramid".

2. Select the method for constructing the base:

     ·     Base center (default) - the base is built along the center and the radius of the inscribed or circumscribed circle.

     ·     Edge - the base is constructed by indicating two points. The length of the edge of the base of the pyramid is the distance between two points.

     ·     Sides - indication of the number of sides of the pyramid. After specifying the number of sides, the system again suggests choosing a construction method (p.2).

3. Specify the necessary parameters depending on the chosen method of building the foundation. The foundation will be built.

CAD software 3D Module 376

4. Choose a way to specify the height of the pyramid:

     ·     Height - indicates the height in the drawing or on the command line.

     ·     DistanceBy2Point - height is calculated by the specified two points in the drawing.

     ·     Axis endpoint - height and direction are calculated at the specified point in the drawing, the first reference point is the center of the base.

     ·     Upper radius - first the radius of the upper base is indicated, then the height is indicated.

5. Specify the required parameters depending on the selected method of specifying the height.

CAD drawing 3D Module 377

6. The pyramid will be built.

CAD drafting 3D Module 378

Grips

1. Grips moving.

2. Grips change height.

3. Grips change the radius of the upper base.

4. Grips change the radius of the lower base.

5. Grips change the radius of the lower base.

CAD software 3D Module 379

3D History

CAD drawing 3D Module 380"3D solid". It is part of the CAD drafting 3D Module 381body.

The following context menu commands are available:

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object and child objects from the tree and model space.

     ·     ShowInDocument - focuses and highlights the object in the center of the model space.

     ·     Rebuild - rearranges the object in the model space.

Wedge

CAD software 3D Module 382Main menu: 3D - Solid - CAD drawing 3D Module 383Wedge.

CAD drafting 3D Module 384Ribbon: 3D Tools - 3D Solids - CAD software 3D Module 385Wedge.

CAD drawing 3D Module 386Toolbar: 3D Solid - CAD drafting 3D Module 387Wedge.

CAD software 3D Module 388Command line: 3DWEDGE.

The command create 3D solid - Wedge.

Procedure

1. Call command  CAD drawing 3D Module 389"Wedge".

2. Select a point of reference (via the context menu or on the command line): "Corner" (default) or "Center".

     ·     Corner - the sides of the wedge are counted from the specified point.

     ·     Center - the sides are counted evenly from the center.

3. Specify the point of reference in the chosen way.

4. Select the method for constructing the base: "Corner" (default), "Cube" or  "Length".

     ·     Corner - a rectangle is constructed when specifying the second point.

     ·     Cube - the length, width and height will be the same and after specifying the point a wedge will be built.

     ·     Length - alternately indicate the length and width of the base.

5. Build the base in the chosen way.

CAD drafting 3D Module 390

6. Select the method of setting the height: "Height" (default) or "DistanceBy2Point".

     ·     Height - the value of the height of the wedge is set in the drawing or in the command line.

     ·     DistanceBy2Point - the value of the height of the wedge is set by specifying two points in the drawing.

7. Specify the height of the selected method.

CAD software 3D Module 391

8. Wedge will be built.

CAD drawing 3D Module 392

Grips

1. Grip move.

2. Grips wedge height changes.

3. Grips change the length or width of the base of the wedge.

4. Grips change the length and width of the base of the wedge.

CAD drafting 3D Module 393

3D History

CAD software 3D Module 394"3D solid". It is part of the CAD drawing 3D Module 395body.

The following context menu commands are available:

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object and child objects from the tree and model space.

     ·     ShowInDocument - focuses and highlights the object in the center of the model space.

     ·     Rebuild - rearranges the object in the model space.

Torus

CAD drafting 3D Module 396Main menu: 3D - Solid - CAD software 3D Module 397Torus.

CAD drawing 3D Module 398Ribbon: 3D Tools - 3D Solids - CAD drafting 3D Module 399Torus.

CAD software 3D Module 400Toolbar: 3D Solid - CAD drawing 3D Module 401Torus.

CAD drafting 3D Module 402Command line: 3DTORUS.

The command create 3D solid - Torus.

Procedure

1. Call command  CAD software 3D Module 403"Torus".

2. Select the method for constructing the axial radius:

     ·     Center (default) - the circle is built in the center and radius.

     ·     3Point - the circle is built at three points.

     ·     RoundBaseBy2Point - build a circle at two points.

     ·     Incircle round base - a circle is constructed along two tangents.

3. Specify the necessary parameters depending on the chosen method of constructing the axial radius.

CAD drawing 3D Module 404

4. Choose a way to specify the cavity radius:

     ·     Minor radius - indicates the radius in the drawing or in the command line.

     ·     DistanceBy2Point - the radius is calculated from the indicated two points in the drawing.

5. Specify the required parameters depending on the selected method of specifying the cavity radius.

CAD drafting 3D Module 405

6. Torus will be built.

CAD software 3D Module 406

Grips

1. Grip move.

2. Grip changes in axial radius.

3. Grips change the radius of the cavity.

CAD drawing 3D Module 407

3D History

CAD drafting 3D Module 408"3D solid". It is part of the CAD software 3D Module 409body.

The following context menu commands are available:

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object and child objects from the tree and model space.

     ·     ShowInDocument - focuses and highlights the object in the center of the model space.

     ·     Rebuild - rearranges the object in the model space.

Polysolid

CAD drawing 3D Module 410Main menu: 3D - Solid - CAD drafting 3D Module 411Polysolid.

CAD software 3D Module 412Ribbon: 3D Tools - 3D Solids - CAD drawing 3D Module 413Polysolid.

CAD drafting 3D Module 414Toolbar: 3D Solid - CAD software 3D Module 415Polysolid.

CAD drawing 3D Module 416Command line: 3DPOLYSOLID.

The command create 3D solid - Polysolid.

Procedure

1. Call command  CAD drafting 3D Module 417"Polysolid".

2. Configure polysolid parameters using the commands:

     ·     Height - specifies the height of the polysolid.

     ·     Width - specifies the width of the polysolid.

     ·     Alignment - alignment is chosen when building: Left, Center or Right.

3. Select the build method:

     ·     Polyline (default) - polysolid will be constructed in the same way as polyline.

     ·     Object - the polysolid will be constructed by specifying the geometric object in the drawing, except for the spline and ellipse.

4. Build polysolid selected method of construction.

CAD software 3D Module 418

Grips

1. Grips height changes

2. Grips change the width.

3. Grips change the width and height.

4. Grips move end points of segments.

5. Grips moving segments.

CAD drawing 3D Module 419

3D History

CAD drafting 3D Module 420"3D solid". It is part of the CAD software 3D Module 421body.

The following context menu commands are available:

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object and child objects from the tree and model space.

     ·     ShowInDocument - focuses and highlights the object in the center of the model space.

     ·     Rebuild - rearranges the object in the model space.

Interfere 3D solids

CAD drawing 3D Module 422Main menu: 3D - Solid - CAD drafting 3D Module 423Interfere 3D solids.

CAD software 3D Module 424Ribbon: 3D Tools - 3D Solids - CAD drawing 3D Module 425Interfere 3D solids.

CAD drafting 3D Module 426Toolbar: 3D Solid - CAD software 3D Module 427Interfere 3D solids.

CAD drawing 3D Module 428Command line: 3DINTERFERE.

Procedure

1. Call command  CAD drafting 3D Module 429"Interfere 3D solids".

2. Select the first set of bodies. To complete the set selection, press "Enter".

CAD software 3D Module 430

2. Select the second set of objects or select the command "check first set". When you select the second set, the overlap between sets, when selecting "check first set", overlaps within the set are analyzed.

CAD drawing 3D Module 431

3. If overlaps exist, a dialog opens "Interference checking", otherwise - the command will end..

CAD drafting 3D Module 432

Interaction objects will be created and highlighted in the drawing.

CAD software 3D Module 433

5. Perform floor analysis. In group "Interfering objects" shows the number of objects from the two sets and the number of pairs found. In group "Highlight" using the buttons "Previous" and "Next" highlight the interaction objects in the drawing. Switch "Delete interference objects on Close" deletes created interaction objects after closing the dialog "Interference checking".

6. Close dialog  "Interference checking" on button "Close".

Extrude

CAD drawing 3D Module 434Main menu: 3D - 3D solid edit - CAD drafting 3D Module 435Extrude.

CAD software 3D Module 436Ribbon: 3D Tools - 3D Solids - CAD drawing 3D Module 437Extrude.

CAD drafting 3D Module 438Toolbar: 3D Edit - CAD software 3D Module 439Extrude.

CAD drawing 3D Module 440Command line: EXTRUDE.

Procedure

1. Call command CAD drafting 3D Module 441"Extrude".

2. Select, if necessary, the type of object being created. Call the command "Mode" from the context menu or from the command line and select type: "Solid" or "Surface".

Solid

Surface

CAD software 3D Module 442

CAD drawing 3D Module 443

3. Select graphic primitives involved in extrusion. To complete the selection, press the key  "Enter".

CAD drafting 3D Module 444

4. Indicate, if necessary, "Taper angle". Call the "Taper angle" command from the context menu or from the command line and enter the angle value. The command can be repeated several times.

CAD software 3D Module 445

5. Select the method for setting the extrusion depth:

     ·     Height (default) - extrusion depth is set by the value in the command line or by the indication in the drawing.

CAD drawing 3D Module 446

     ·     Direction - extrusion depth is set by two points in the drawing. The direction should not be coplanar or tangent to the plane of the object.

CAD drafting 3D Module 447CAD software 3D Module 448

     ·     Path - extrusion depth is set by specifying the trajectory. The path must not be coplanar or tangent to the plane of the object.

CAD drawing 3D Module 449CAD drafting 3D Module 450

6. Set the extrusion depth using the selected method. The body or surface will be built.

CAD software 3D Module 451

Grips

1. Grip taper - allows you to change the angle of taper.

2. Grip Depth - allows you to change the depth of extrusion.

3. Grips section - handles change the shape of the section.

CAD drawing 3D Module 452

Revolve

CAD drafting 3D Module 453Main menu: 3D - 3D solid edit - CAD software 3D Module 454Revolve.

CAD drawing 3D Module 455Ribbon: 3D Tools - 3D Solids - CAD drafting 3D Module 456Revolve.

CAD software 3D Module 457Toolbar: 3D Edit - CAD drawing 3D Module 458Revolve.

CAD drafting 3D Module 459Command line: REVOLVE.

Procedure

1. Call command CAD software 3D Module 460"Revolve".

2. Select, if necessary, the type of object being created. Call the command "Mode" from the context menu or from the command line and select type: "Solid" or "Surface".

Solid

Surface

CAD drawing 3D Module 461

CAD drafting 3D Module 462

3. Select rotating graphic primitives. To complete the selection, press the "Enter" key.

CAD software 3D Module 463

4. Select rotation axis:

2Points (default) - the axis is selected by sequential indication of two points.

Object - the axis is selected by specifying the object.

X/Y/Z - UCS axes are selected as the axis.

CAD drawing 3D Module 464

5. Change, if necessary, the direction of rotation. Call the command "Reverse" from the context menu or from the command line. Repeat the command the required number of times.

6. Change, if necessary, the initial angle of reference. Call the command "Specify start angle" from the context menu or from the command line. Enter the value of the starting angle. The value may be negative. Repeat the command the required number of times.

7. Specify the angle of rotation. The body or surface will be built.

CAD drafting 3D Module 465

Grips

1. Grip rotation angle - allows you to change the rotation angle.

2. Grip axis movement - allows you to change the position of the axis.

3. Grips section - handles change the shape of the section.

CAD software 3D Module 466

Loft

CAD drawing 3D Module 467Main menu: 3D - 3D solid edit - CAD drafting 3D Module 468Loft.

CAD software 3D Module 469Ribbon: 3D Tools - 3D Solids - CAD drawing 3D Module 470Loft.

CAD drafting 3D Module 471Toolbar: 3D Edit - CAD software 3D Module 472Loft.

CAD drawing 3D Module 473Command line: LOFT.

Procedure

1. Call command CAD drafting 3D Module 474"Loft".

2. Select, if necessary, the type of object being created. Call the command "Mode" from the context menu or from the command line and select type: "Solid" or "Surface".

Solid

Surface

CAD software 3D Module 475

CAD drawing 3D Module 476

3. Specify the sections in sequence in the required order. To complete, press the "Enter" key. All sections must be either closed or open.

CAD drafting 3D Module 477

4. Set additional build parameters:

Cross-section only (default) - only sections are taken into account when calculating stretching.

CAD software 3D Module 478CAD drawing 3D Module 479

Guides - when calculating the stretching, sections and additional guides are taken into account.

CAD drafting 3D Module 480CAD software 3D Module 481

Path - when calculating the extrusion takes into account the section and the trajectory

CAD drawing 3D Module 482CAD drafting 3D Module 483

5. Confirm the parameters on the "Enter" key. Loft will be built.

CAD software 3D Module 484

Grips

Section Grips - allow you to change the shape of sections.

CAD drawing 3D Module 485

Sweep

CAD drafting 3D Module 486Main menu: 3D - 3D solid edit - CAD software 3D Module 487Sweep.

CAD drawing 3D Module 488Ribbon: 3D Tools - 3D Solids - CAD drafting 3D Module 489Sweep.

CAD software 3D Module 490Toolbar: 3D Edit - CAD drawing 3D Module 491Sweep.

CAD drafting 3D Module 492Command line: SWEEP.

Procedure

1. Call command CAD software 3D Module 493"Sweep".

2. Select, if necessary, the type of object being created. Call the command "Mode" from the context menu or from the command line and select type: "Solid" or "Surface".

Solid

Surface

CAD drawing 3D Module 494

CAD drafting 3D Module 495

3. Select graphic primitives involved in the shift. To complete the selection, press the "Enter" key.

CAD software 3D Module 496

4. If necessary, specify the alignment. Alignment can be perpendicular to the path or parallel to the section. Call the command "Alignment" from the context menu or from the command line and select the alignment option.

5. If necessary, specify a base point. The trajectory and section will be combined at the base point. Call the command "Base point" from the context menu or from the command line and specify the point on the section.

6. If necessary, specify the scale. Call the "Scale" command from the context menu or from the command line and specify the scale value.

7. If necessary, specify the twist angle. Call the "Twist" command from the context menu or from the command line and specify the angle value.

8. Select the trajectory.

CAD drawing 3D Module 497

9. Sweep will be built.

CAD drafting 3D Module 498

Grips

1. Grip move - allows you to move the 3D-body.

CAD software 3D Module 499

Slice

CAD drawing 3D Module 500Main menu: 3D - 3D solid edit - CAD drafting 3D Module 501Slice.

CAD software 3D Module 502Ribbon: 3D Tools - 3D Solids - CAD drawing 3D Module 503Slice.

CAD drafting 3D Module 504Toolbar: 3D Edit - CAD software 3D Module 505Slice.

CAD drawing 3D Module 506Command line: SLICE.

Procedure

1. Call command CAD drafting 3D Module 507"Slice".

2. Select the 3D body to be cut. To complete the selection, press the "Enter" key.

CAD software 3D Module 508

3. Select the method of defining the section plane:

2Points (default) - a cutting plane is constructed at two points perpendicular to the XY plane.

3Points - the cutting plane is defined by three points.

Planar object - A flat object is selected as the cutting plane.

4. Build a cutting plane in the chosen way.

CAD drawing 3D Module 509

5. Click the side you want to leave, or "Both".

6. The selected 3D bodies will be cut.

CAD drafting 3D Module 510

Section

CAD software 3D Module 511Main menu:  3D - 3D solid edit - CAD drawing 3D Module 512Section.

CAD drafting 3D Module 513Ribbon: 3D Tools - 3D Solids - CAD software 3D Module 514Section.

CAD drawing 3D Module 515Toolbar: 3D Edit - CAD drafting 3D Module 516Section.

CAD software 3D Module 517Command line: SECTION.

The command creates a region object representing a 2D cross section of 3D objects, including 3D solids, surfaces, and meshes.

Procedure

1. Prepare objects.

CAD drawing 3D Module 518CAD drafting 3D Module 519

2. Call command CAD software 3D Module 520"Section".

3. Select one or more 3D objects. Selecting multiple objects results in a separate area for each object.

CAD drawing 3D Module 521

4. Choose a method for specifying the plane:

     ·     3points (default) - Specifies a cutting plane by three points.

CAD drafting 3D Module 522CAD software 3D Module 523

     ·     Object - Aligns a cutting plane with a segment, circle, ellipse, circular or elliptical arc, 2D spline, or 2D polyline segment.

CAD drawing 3D Module 524CAD drafting 3D Module 525

     ·     Zaxis - Defines a section plane by specifying one point on that section plane and a second point on the z-axis or normal on that plane.

1. Point on the cutting plane. Sets the first point on the plane.

2. A point on the Z-axis (normal) on the plane. Sets the point that defines the axis perpendicular to the plane.

CAD software 3D Module 526

     ·     View - Aligns the section plane with respect to the current view. After choosing the method, you should specify the point through which the plane will pass.

Point 0,0,0

CAD drawing 3D Module 527

Point 20,20,20

CAD drafting 3D Module 528

     ·     XY - Aligns the section plane with the XY plane of the current UCS. After choosing the method, you should specify the point through which the plane will pass.

CAD software 3D Module 529

     ·     YZ - Aligns the section plane with the YZ plane of the current UCS. After choosing the method, you should specify the point through which the plane will pass.

CAD drawing 3D Module 530

     ·     ZX - Aligns the section plane with the ZX plane of the current UCS. After choosing the method, you should specify the point through which the plane will pass.

CAD drafting 3D Module 531

5. In accordance with the selected method, specify the section plane.

6. The area will be built.

Grips

1. Mode change grip: move mode, area change mode.

2. Nodal grips.

3. Movement grip.

CAD software 3D Module 532CAD drawing 3D Module 533

 

Thicken

CAD drafting 3D Module 534Main menu: 3D - 3D solid edit - CAD software 3D Module 535Thicken.

CAD drawing 3D Module 536Ribbon: 3D Tools - 3D Solids - CAD drafting 3D Module 537Thicken.

CAD software 3D Module 538Toolbar: 3D Edit - CAD drawing 3D Module 539Thicken.

CAD drafting 3D Module 540Command line: THICKEN.

The team works with "Surface" objects. The command sets the surface thickness.

Procedure

1. Call command CAD software 3D Module 541"Thicken".

2. Select surfaces to set the thickness. To complete the selection, press the "Enter" key.

CAD drawing 3D Module 542

3. Enter a new thickness. The value may be negative.

CAD drafting 3D Module 543

Presspull

CAD software 3D Module 544Main menu: 3D - 3D solid edit - CAD drawing 3D Module 545Presspull.

CAD drafting 3D Module 546Ribbon: 3D Tools - 3D Solids - CAD software 3D Module 547Presspull.

CAD drawing 3D Module 548Toolbar: 3D Edit - CAD drafting 3D Module 549Presspull.

CAD software 3D Module 550Command line: PRESSPULL.

Procedure

1. Call command CAD drawing 3D Module 551"Presspull".

2. Select a face or limited area.

CAD drafting 3D Module 552

3. Use the "Multiple" context menu command if you need to specify multiple areas.

4. Set the extrusion distance. The value may be negative.

5. Extrusion of the face (closed area) will be performed.

CAD software 3D Module 553

Xedges

CAD drawing 3D Module 554Main menu: 3D - 3D solid edit - CAD drafting 3D Module 555Xedges.

CAD software 3D Module 556Ribbon: 3D Tools - 3D Solids - CAD drawing 3D Module 557Xedges.

CAD drafting 3D Module 558Toolbar: 3D Edit - CAD software 3D Module 559Xedges.

CAD drawing 3D Module 560Command line: XEDGES.

Procedure

CAD drafting 3D Module 561

1. Call command CAD software 3D Module 562"Xedges".

2. Specify the 3D body from which you want to extract faces.

3. Faces will be extracted. The team will continue to work in a cyclical mode. To exit the cyclic mode, press the "Esc" key.

CAD drawing 3D Module 563

Offset edge

CAD drafting 3D Module 564Main menu: 3D - 3D solid edit - CAD software 3D Module 565Offset edge.

CAD drawing 3D Module 566Ribbon: 3D Tools - 3D Solids - CAD drafting 3D Module 567Offset Edge.

CAD software 3D Module 568Toolbar: 3D Edit - CAD drawing 3D Module 569Offset edge.

CAD drafting 3D Module 570Command line: OFFSETEDGE.

Procedure

1. Call command CAD software 3D Module 571"Offset edge".

2. Specify the edge of the 3D body on which the contour will be built.

CAD drawing 3D Module 572

3. Specify the shape of the contour corners. Call the "Corner" command from the context menu or from the command line and select "Round" or "Sharp". The radius of the round corners is equal to the size of the contour shift.

CAD drafting 3D Module 573

4. Specify the size of the contour shift. Call the command "Distance" from the context menu or from the command line and set the value.

5. Pick a point defining the side of the contour offset.

6. The contour of the face will be built.

CAD software 3D Module 574

 

Fillet edge

CAD drawing 3D Module 575Main menu: 3D - 3D solid edit - CAD drafting 3D Module 576Fillet edge.

CAD software 3D Module 577Ribbon: 3D Tools - 3D Solids - CAD drawing 3D Module 578Fillet Edge.

CAD drafting 3D Module 579Toolbar: 3D Edit - CAD software 3D Module 580Fillet edge.

CAD drawing 3D Module 581Command line: FILLETEDGE.

Procedure

1. Call command CAD drafting 3D Module 582"Fillet edge".

2. Set the blend radius. Call the "Radius" command from the context menu or from the command line and specify the radius value.

3. Select the method for specifying the edges:

     ·     Edge (default) - edges are selected by sequential selection.

     ·     Loop - first one edge of the desired edge is selected, then the edge. All edges of the desired face are added to the set.

4. Specify edges in the selected way. All edges must have an adjacent face. To complete the selection, press the "Enter" key.

CAD software 3D Module 583

5. Check the resulting pairing. If necessary, change the radius.

6. Press the "Enter" key to confirm. Edge mate will be built.

CAD drawing 3D Module 584

Chamfer edge

CAD drafting 3D Module 585Main menu: 3D - 3D solid edit - CAD software 3D Module 586Chamfer edge.

CAD drawing 3D Module 587Ribbon: 3D Tools - 3D Solids - CAD drafting 3D Module 588Chamfer Edge.

CAD software 3D Module 589Toolbar: 3D Edit - CAD drawing 3D Module 590Chamfer edge.

CAD drafting 3D Module 591Command line: CHAMFEREDGE.

Procedure

1. Call command CAD software 3D Module 592"Chamfer edge".

2. Set the bevel distance. Call the "Distance" command from the context menu or from the command line and specify the distance value.

3. Select the method for specifying the edges:

     ·     Edge (default) - edges are selected by sequential selection.

     ·     Loop - first one edge of the desired edge is selected, then the edge. All edges of the desired face are added to the set.

4. Specify edges in the selected way. All edges must have an adjacent face. To complete the selection, press the "Enter" key.

CAD drawing 3D Module 593

5. Check the chamfer. If necessary, change the distance.

6. Press the "Enter" key to confirm. Chamfer edge will be built.

CAD drafting 3D Module 594

Solid editing

CAD software 3D Module 595Main menu: 3D - 3D solid edit - CAD drawing 3D Module 596Solidedit.

CAD drafting 3D Module 597Ribbon: 3D Tools - 3D Solids - CAD software 3D Module 598Solid Editing.

CAD drawing 3D Module 599Toolbar: 3D Edit - CAD drafting 3D Module 600Solidedit.

CAD software 3D Module 601Command line: SOLIDEDIT.

The team edits 3D solid, its faces and edges.

Procedure

1. Call command CAD drawing 3D Module 602"Solidedit".

2. Select the type of object to edit: Edge, Face, Body. For each type of object editing its menu of commands. To return the selection of the type of object being edited, press the "Enter" key.

3. Perform editing using the context menu commands:

     ·     Color (Edge, Face) - command sets new color.

                 ·     Select the faces (edges) on which you want to change the color. To complete the selection, press the "Enter" key. Open dialog "Select color".

CAD drafting 3D Module 603

                 ·     In the "Select color" dialog box, define a new color in the way you like and click the "OK" button.

CAD software 3D Module 604

                 ·     New color will be applied.

CAD drawing 3D Module 605

Note:

The change in the color of the edges can be seen on the visual styles with the edges shown.

When you change the color of the face, the colors of its edges change.

     ·     Copy (Edge, Face) - allows you to copy a face (edge).

                 ·     Select the faces (edges) on which you want to change the color. To complete the selection, press the "Enter" key.

CAD drafting 3D Module 606

                 ·     Specify the base copy point.

CAD software 3D Module 607

                 ·     Specify the end point to which the faces (edges) will be copied.

CAD drawing 3D Module 608

                 ·     Copy will be made. The face is copied as a region, the edge is a segment.

CAD drafting 3D Module 609

     ·     Imprint (Body) - command action is similar to command action  "Imprint".

     ·     Separate (body) - command shares a body that has several kinks.

Select body. The body will be divided in the presence of kinks.

4. Use the editing commands of the selected object type (p. 3) the required number of times. To return to the choice of the type of object being edited (p. 2), press the "Enter" key.

5. The "Solidedit" command works in a cyclic mode. To end the command, press the "Esc" key.

Sheet modeling

Sheet solid

Important!

This functionality requires a C3D 3D modeling engine.

CAD software 3D Module 610Main menu: 3D - Sheet metal - CAD drawing 3D Module 611Sheet metal.

CAD drafting 3D Module 612Ribbon: 3D Tools - Sheet solids - CAD software 3D Module 613Sheet metal.

CAD drawing 3D Module 614Toolbar: Sheet metal - CAD drafting 3D Module 615Sheet metal.

CAD software 3D Module 616Command line: SMCREATE.

The shape of the sheet solid is determined by its sketch. The order in which the sheet solid is drawn depends on whether the sketch is closed or open.

Procedure

1. Draw a sketch: Closed or Open.

A closed sketch is extruded by a specified thickness in a direction perpendicular to its plane.

The following can act as a closed contour: closed polylines, circles, ovals.

CAD drawing 3D Module 617

An open sketch is extruded to one or both sides by a specified distance; the thickness is added to the resulting surface. Sketch lines form flat sections of a sheet solid, arcs form bends of corresponding radius, and contour corners form bends with a user-defined inner radius.

The following can act as an open contour: open polylines with straight sections, lines, arcs.

CAD drafting 3D Module 618

2. Call command Sheet solid. The CAD software 3D Module 619"Sheet solid" dialog will open.

CAD drawing 3D Module 620

3. Select a sketch. A red cursorCAD drafting 3D Module 621 means that the sketch selection mode is on. If a sketch is not selected, the corresponding red "Sketch is not selected" is displayed.

CAD software 3D Module 622

If you need to replace the sketch (select another), re-enter the sketch selection mode by clicking the CAD drawing 3D Module 623"Sketch" button..

4. Specify the required parameters. Depending on the type of sketch, the composition of the parameters will change.

Open

Close

CAD drafting 3D Module 624

CAD software 3D Module 625

Confirm the action on the "OK" button. The sheet body will be built. If the "OK" button is grayed out, it means that the sketch was not selected or the parameters were set incorrectly. In the "3d History", a CAD drawing 3D Module 626"Sheet metal" object containing a sketch will be created with reference to an existing or new body.

CAD drafting 3D Module 627

Dialog

CAD software 3D Module 628

Button CAD drawing 3D Module 629"Sketch" - turns on the sketch selection mode in the drawing.

Field "Thickness" - sheet body thickness.

Field "Distance" - sheet body length, if a closed sketch is specified, the field defines the thickness of the sheet body.

Field "Distance 2" - the length of the sheet body when the direction "Both directions" is selected, if a closed sketch is specified, the field determines the thickness of the sheet body.

Direction select switch group:

     ·     CAD drafting 3D Module 630Forward direction - directs the extrusion toward the positive direction of the axis perpendicular to the sketch plane.

     ·     CAD software 3D Module 631Reverse direction - directs the extrusion toward the negative direction of the axis perpendicular to the sketch plane. 

     ·     CAD drawing 3D Module 632Both direction - directs the extrusion to both sides of the sketch plane, the distances are determined by the "Distance" and "Distance 2" parameters.

     ·     CAD drafting 3D Module 633Middle plane - directs the extrusion to both sides of the sketch plane at the same distance.

Field "Coefficient" - neutral layer coefficient.

Field "Radius" - radius of connection of straight sections.

3D History

CAD software 3D Module 634"Sheet metal". As part of the CAD drawing 3D Module 635 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drafting 3D Module 636.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Shell

Important!

This functionality requires a C3D 3D modeling engine.

CAD software 3D Module 637Main menu: 3D - Sheet metal - CAD drawing 3D Module 638Shell.

CAD drafting 3D Module 639Ribbon: 3D Tools - Sheet solids - CAD software 3D Module 640Shell.

CAD drawing 3D Module 641Toolbar: Sheet metal - CAD drafting 3D Module 642Shell.

CAD software 3D Module 643Command line: SMSHELL.

The sectional shape of the shell is determined by its sketch. A simple shell is formed by extruding a sketch in a direction perpendicular to its plane and adding thickness to the resulting surface. A sketch outline can be closed or open. If the contour is closed, then the shell is cut in height, the location and size of the gap are specified by the user. Various methods of trimming the shell edges are possible.

Sketch lines form flat portions of the shell, and contour corners form bends with a user-defined radius.

Procedure

1. Draw a sketch. The sketch can be closed or open.

The following can act as a closed contour: closed polylines, circles, ovals.

An open contour can be: open polylines, lines, arcs, open splines.

CAD drawing 3D Module 644

2. Call command CAD drafting 3D Module 645"Shell". The "Shell" dialog will open.

CAD software 3D Module 646

3. Select a sketch. A red cursorCAD drawing 3D Module 647 means that the sketch selection mode is on. If a sketch is not selected, the corresponding red "Sketch is not selected" is displayed.

CAD drafting 3D Module 648

If you need to replace the sketch (select another), re-enter the sketch selection mode by clicking the CAD software 3D Module 649"Sketch" button.

4. Specify the required parameters. Depending on the type of sketch, the composition of the parameters will change. For a contour with arcs, the segmentation options become available.

CAD drawing 3D Module 650

5. Confirm the action with the "OK" button. The sheet solid will be built. If the "OK" button is grayed out, it means that the sketch was not selected or the parameters were set incorrectly. In "3d History", a CAD drafting 3D Module 651"Shell" object containing the sketch will be created and snapped to an existing or new solid.

CAD software 3D Module 652

Dialog

CAD drawing 3D Module 653

3D History

CAD drafting 3D Module 654"Shell". As part of the CAD software 3D Module 655 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drawing 3D Module 656.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Ruled shell

Important!

This functionality requires a C3D 3D modeling engine.

CAD drafting 3D Module 657Main menu: 3D - Sheet metal - CAD software 3D Module 658Ruled shellSheet metal.

CAD drawing 3D Module 659Ribbon: 3D Tools - Sheet solids - CAD drafting 3D Module 660Ruled shellа.

CAD software 3D Module 661Toolbar: Sheet metal - CAD drawing 3D Module 662Ruled shell.

CAD drafting 3D Module 663Command line: SMRULEDSHELL.

The sectional shape of the shell is determined by its sketch. Two sketches are required for the construction of the ruled shell. A sketch outline can be closed or open. If the contour is closed, then the shell is cut in height, the location and size of the gap are specified by the user. Various methods of trimming the shell edges are possible.

Procedure

1. Draw 2 sketches. The sketch can be closed or open.

The following can act as a closed contour: closed polylines, circles, ovals.

An open contour can be: open polylines, lines, arcs, open splines.

CAD software 3D Module 664

2. Call command CAD drawing 3D Module 665"Ruled shell". The "Ruled shell" dialog will open.

3. Select 2 sketches. A red cursor CAD drafting 3D Module 666 means that the sketch selection mode is on. If no sketches are selected, the corresponding red text "Sketch 1, Sketch 2 are not selected" is displayed.

CAD software 3D Module 667CAD drawing 3D Module 668

If you need to replace the sketch (select another), re-enter sketch selection mode by pressing the CAD drafting 3D Module 669"Sketch 1" or CAD software 3D Module 670"Sketch 2" button.

4. Specify the required parameters.

5. Confirm the action with the "OK" button. The ruled shell will be built. If the "OK" button is grayed out, it means that no sketches were selected or the parameters were set incorrectly. In "3d History", a CAD drawing 3D Module 671"Ruled shell" object containing sketches will be created and snapped to an existing or new solid.

 

CAD drafting 3D Module 672

Dialog

CAD software 3D Module 673

3D History

CAD drawing 3D Module 674"Ruled shell". As part of the CAD drafting 3D Module 675 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD software 3D Module 676.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Plate

Important!

 

This functionality requires a C3D 3D modeling engine.

CAD drawing 3D Module 677Main menu: 3D - Sheet metal - CAD drafting 3D Module 678Plate.

CAD software 3D Module 679Ribbon: 3D Tools - Sheet solids - CAD drawing 3D Module 680Plate.

CAD drafting 3D Module 681Toolbar: Sheet metal - CAD software 3D Module 682Plate.

CAD drawing 3D Module 683Command line: SMPLATE.

A plate is a flat sheet metal piece glued to a sheet metal piece. The plate is formed by extruding a closed sketch. The extrusion depth can be arbitrary or equal to the thickness of the sheet metal.

Procedure

1. Draw a closed loop sketch. The sketch must be positioned on the outer or inner planar face of the sheet solid.

CAD drafting 3D Module 684

2. Call command CAD software 3D Module 685"Plate". The "Plate" dialog will open.

CAD drawing 3D Module 686

3. Select a sketch. A red cursorCAD drafting 3D Module 687 means that the sketch selection mode is on. If a sketch is not selected, the corresponding red "Sketch is not selected" is displayed.

CAD software 3D Module 688

If you need to replace the sketch (select another), re-enter the sketch selection mode by clicking the CAD drawing 3D Module 689"Sketch" button.

4. Specify the required parameters.

5. Confirm the action with the "OK" button. The sheet solid will be built. If the "OK" button is grayed out, it means that the sketch was not selected or the parameters were set incorrectly. In "3d History", a CAD drafting 3D Module 690"Plate" object containing the sketch will be created and snapped to an existing or new solid.

CAD software 3D Module 691

Dialog

CAD drawing 3D Module 692

Button CAD drafting 3D Module 693"Sketch" - turns on the sketch selection mode in the drawing.

Field "Thickness" - plate thickness.

Switch "In thickness" - when the switch is on, the thickness of the plate is equal to the thickness of the sheet, the "Thickness" field is hidden.

3D History

CAD software 3D Module 694"Plate". As part of the CAD drawing 3D Module 695 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drafting 3D Module 696.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Bend along edge

Important!

This functionality requires a C3D 3D modeling engine.

CAD software 3D Module 697Main menu: 3D - Sheet metal - CAD drawing 3D Module 698Bend along edge.

CAD drafting 3D Module 699Ribbon: 3D Tools - Sheet solids - CAD software 3D Module 700Bend along edge.

CAD drawing 3D Module 701Toolbar: Sheet metal - CAD drafting 3D Module 702Bend along edge.

CAD software 3D Module 703Command line: SMEDGE.

A bend is created along one or more edges of the sheet metal. The edge (s) must be straight and belong to the outer or inner flat face of the sheet metal.

Procedure

1. Call command CAD drawing 3D Module 704"Bend along edge". The "Bend along edge" dialog will open.

CAD drafting 3D Module 705

2. Select an edge. Red cursor CAD software 3D Module 706 means selection mode is on. If an edge is not selected, the corresponding red text "Ribs are not selected" is displayed.

CAD drawing 3D Module 707CAD drafting 3D Module 708

If you need to remove or add an edge, enter the selection mode again by pressing theCAD software 3D Module 709"Ribs" button. Selected edges are highlighted in red, re-selecting an edge removes the selection.

CAD drawing 3D Module 710CAD drafting 3D Module 711

3. Specify the required parameters.

CAD software 3D Module 712

4. Confirm the action with the "OK" button. The bend will be built. If the "OK" button is inactive, it means that an edge was not selected or the parameters were set incorrectly. A CAD drawing 3D Module 713"Bend along edge" object will be created in "3d History" and will snap to an existing or new solid.

CAD drafting 3D Module 714

Dialog

CAD software 3D Module 715

Button CAD drawing 3D Module 716"Ribs" - turns on the ribs selection mode in the drawing.

Common

CAD drafting 3D Module 717

Continuation of the bend

CAD software 3D Module 718

Angle and radius

CAD drawing 3D Module 719

Location of the bend

CAD drafting 3D Module 720

Lateral face

CAD software 3D Module 721CAD drawing 3D Module 722

Closing corners

CAD drafting 3D Module 723

Freeing

CAD software 3D Module 724

3D History

CAD drawing 3D Module 725"Bend along edge". As part of the CAD drafting 3D Module 726 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD software 3D Module 727.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Bend by sketch

Important!

 

This functionality requires a C3D 3D modeling engine.

CAD drawing 3D Module 728Main menu: 3D - Sheet metal - CAD drafting 3D Module 729Fold by sketch.

CAD software 3D Module 730Ribbon: 3D Tools - Sheet solids - CAD drawing 3D Module 731Fold by sketch.

CAD drafting 3D Module 732Toolbar: Sheet metal - CAD software 3D Module 733Fold by sketch.

CAD drawing 3D Module 734Command line: SMJOINTBEND.

Fold by sketch - A multi-bend feature whose profile is defined by a contour in a sketch. The corners of a path in a sketch form bends with a user-defined inner radius.

Procedure

1. Draw a sketch. The bend should be located along one straight edge or chain of straight edges of the sheet metal part. The edge is the bend line, and the containing face (outside or inside) is the base face of the bend.

CAD drafting 3D Module 735

2. Call command CAD software 3D Module 736"Fold by sketch". The "Fold by sketch" dialog will open.

CAD drawing 3D Module 737

3. Select the sketch (path) and the edge of the sheet solid. Red cursor CAD drafting 3D Module 738 means selection mode is on.

If the path and edge of the sheet solid are not selected, the corresponding red "Sketch and an edge are not selected" text box is displayed.

CAD software 3D Module 739CAD drawing 3D Module 740CAD drafting 3D Module 741

Pick multiple edges of the sheet body, if necessary.

CAD software 3D Module 742

Press theCAD drawing 3D Module 743"Sketch and an edge" button to complete your selection.

If you need to replace or add objects, enter the selection mode again by pressing the CAD drafting 3D Module 744"Sketch and an edge" button.

4. Specify the required parameters.

5. Confirm the action with the "OK" button. The fold by sketch will be constructed. If the "OK" button is grayed out, it means that the path and edges were not selected or the parameters were set incorrectly. In "3d History", a CAD software 3D Module 745"Fold by Sketch" object is created that contains the sketch and snapped to an existing or new solid.

CAD drawing 3D Module 746

Dialog

CAD drafting 3D Module 747

3D History

CAD software 3D Module 748"Fold by sketch". As part of the CAD drawing 3D Module 749 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drafting 3D Module 750.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Bend along line

Important!

This functionality requires a C3D 3D modeling engine.

CAD software 3D Module 751Main menu: 3D - Sheet metal - CAD drawing 3D Module 752Bend along line.

CAD drafting 3D Module 753Ribbon: 3D Tools - Sheet solids - CAD software 3D Module 754Bend along line.

CAD drawing 3D Module 755Toolbar: Sheet metal - CAD drafting 3D Module 756Bend along line.

CAD software 3D Module 757Command line: SMOVERSEG.

A sheet metal part can be bent in a straight line relative to the outer or inner flat face of that part. The specified line and face will be the bend line and bend base face.

Procedure

1. Draw a bend line. The line can be a separate primitive or part of a sketch. The bend line must intersect the body completely.

CAD drawing 3D Module 758

2. Call command CAD drafting 3D Module 759"Bend along line". The "Bend along line" dialog will open.

CAD software 3D Module 760

3. Select the face and bend line. Red cursorCAD drawing 3D Module 761 means selection mode is on. If faces and bend line are not selected, the corresponding red text "Faces and fold line are not selected" is displayed.

CAD drafting 3D Module 762CAD software 3D Module 763

If you need to replace a face (select a different one), re-enter sketch selection mode by clicking the CAD drawing 3D Module 764"Faces and fold line" button.

4. Specify the required parameters.

5. Confirm the action with the "OK" button. The bend will be constructed. If the "OK" button is inactive, it means that no objects were selected or the parameters were set incorrectly. In "3d History", a CAD drafting 3D Module 765"Bend along line" object containing the sketch will be created and snapped to an existing or new solid.

CAD software 3D Module 766

Dialog

CAD drawing 3D Module 767

3D History

CAD drafting 3D Module 768"Bend along line". As part of the CAD software 3D Module 769 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drawing 3D Module 770.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Jog

Important!

This functionality requires a C3D 3D modeling engine.

CAD drafting 3D Module 771Main menu: 3D - Sheet metal - CAD software 3D Module 772Jog.

CAD drawing 3D Module 773Ribbon: 3D Tools - Sheet solids - CAD drafting 3D Module 774Jog.

CAD software 3D Module 775Toolbar: Sheet metal - CAD drawing 3D Module 776Jog.

CAD drafting 3D Module 777Command line: SMJOG.

Procedure

1. Draw a bend line. The line can be a separate primitive or part of a sketch. The bend line must intersect the body completely.

CAD software 3D Module 778

2. Call command CAD drawing 3D Module 779"Jog". The "Jog" dialog will open

CAD drafting 3D Module 780

3. Select the face and bend line. Red cursorCAD software 3D Module 781 means selection mode is on. If faces and bend line are not selected, the corresponding red text "Faces and fold line are not selected" is displayed.

 

CAD drawing 3D Module 782CAD drafting 3D Module 783

If you need to replace a face (select a different one), re-enter sketch selection mode by clicking the CAD software 3D Module 784"Faces and fold line" button.

4. Specify the required parameters.

5. Confirm the action with the "OK" button. The Jog the line will be constructed. If the "OK" button is inactive, it means that no objects were selected or the parameters were set incorrectly. In "3d History", a CAD drawing 3D Module 785"Jog" object will be created containing the sketch and will snap to an existing or new body.

CAD drafting 3D Module 786

Dialog

CAD software 3D Module 787

3D History

CAD drawing 3D Module 788"Jog". As part of the CAD drafting 3D Module 789 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD software 3D Module 790.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Closing corners

Important!

 

This functionality requires a C3D 3D modeling engine.

CAD drawing 3D Module 791Main menu: 3D - Sheet metal - CAD drafting 3D Module 792 Closing corners.

CAD software 3D Module 793Ribbon: 3D Tools - Sheet solids - CAD drawing 3D Module 794 Closing corners.

CAD drafting 3D Module 795Toolbar: Sheet metal - CAD software 3D Module 796 Closing corners.

CAD drawing 3D Module 797Command line: SMCORNER.

Procedure

1. Call command CAD drafting 3D Module 798"Closing corners". The "Closing corners" dialog will open.

CAD software 3D Module 799

2. Select a bend angle. Red cursor CAD drawing 3D Module 800 means selection mode is on.

CAD drafting 3D Module 801

If you need to change the angle (select another), enter the selection mode again by pressing the CAD software 3D Module 802"Angle of bend" button.

3. Specify the required parameters.

CAD drawing 3D Module 803

4. Confirm the action with the "OK" button. The closing corners will be constructed. If the "OK" button is inactive, it means that the corner was not selected or the parameters were set incorrectly. In the "3d History" object CAD drafting 3D Module 804"Closing corners" will be created, with a connection to an existing or new body.

CAD software 3D Module 805

Dialog

CAD drawing 3D Module 806

3D History

CAD drafting 3D Module 807"Closing corners". As part of the CAD software 3D Module 808 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drawing 3D Module 809.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Hole

Important!

This functionality requires a C3D 3D modeling engine.

CAD drafting 3D Module 810Main menu: 3D - Sheet metal - CAD software 3D Module 811Hole.

CAD drawing 3D Module 812Ribbon: 3D Tools - Sheet solids - CAD drafting 3D Module 813Hole.

CAD software 3D Module 814Toolbar: Sheet metal - CAD drawing 3D Module 815Hole.

CAD drafting 3D Module 816Command line: SMHOLE.

Procedure

1. Draw a closed sketch on one of the faces of the sheet solid.

CAD software 3D Module 817

2. Call command CAD drawing 3D Module 818"Hole". The "Hole" dialog will open.

CAD drafting 3D Module 819

3. Select a sketch. A red cursor CAD software 3D Module 820 means that the sketch selection mode is on. If a sketch is not selected, the corresponding red "Sketch is not selected" is displayed.

CAD drawing 3D Module 821

If you need to replace the sketch (select another), re-enter the sketch selection mode by clicking the CAD drafting 3D Module 822"Sketch" button.

4. Specify the required parameters.

CAD software 3D Module 823

5. Confirm the action with the "OK" button. The hole will be built. If the "OK" button is grayed out, it means that the sketch was not selected or the parameters were set incorrectly. In "3d History", a CAD drawing 3D Module 824"Hole" object containing a sketch will be created and snapped to an existing or new solid.

CAD drafting 3D Module 825

Dialog

CAD software 3D Module 826

Button CAD drawing 3D Module 827"Sketch" - turns on the sketch selection mode in the drawing.

Switch "Cutting" - defines the clipping area. When the switch is on, the area inside the sketch is cut out, when it is off - outside.

Switch "In thickness" - defines the depth of the cut. When the switch is on, the cut is made to the thickness of the sheet, when it is off, it is set independently.

Switch "Invert direction" - changes the direction of the cut.

Field "Thickness" - depth of cut, the field is active when the "In thickness" switch is off.

3D History

CAD drafting 3D Module 828"Hole". As part of the CAD software 3D Module 829 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drawing 3D Module 830.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Unbend

Important!

This functionality requires a C3D 3D modeling engine.

CAD drafting 3D Module 831Main menu: 3D - Sheet metal - CAD software 3D Module 832Unbend.

CAD drawing 3D Module 833Ribbon: 3D Tools - Sheet solids - CAD drafting 3D Module 834Unbend.

CAD software 3D Module 835Toolbar: Sheet metal - CAD drawing 3D Module 836Unbend.

CAD drafting 3D Module 837Command line: SMUNBEND.

The command allows you to unbend sections of a sheet body.

Procedure

1. Call command CAD software 3D Module 838"Unbend". The "Unbend" dialog will open.

CAD drawing 3D Module 839

2. Select the face in the plane of which the bend will be performed and the bend adjacent to the face. Red cursorCAD drafting 3D Module 840 means selection mode is on. If no faces are selected, the corresponding red "Fixed face and bend faces are not selected" text is displayed.

CAD software 3D Module 841CAD drawing 3D Module 842

If you need to replace a face or add faces, re-enter selection mode by pressing the CAD drafting 3D Module 843"Fixed face and bend faces" button. To confirm your choice, click on CAD software 3D Module 844.

CAD drawing 3D Module 845CAD drafting 3D Module 846

3. Confirm the action with the "OK" button. The sheet solid will be unbent. If the "OK" button is grayed out, then no faces were selected. An CAD software 3D Module 847"Unbend" object will be created in the "3d History", with a connection to an existing or new body.

Dialog

CAD drawing 3D Module 848

Button CAD drafting 3D Module 849"Fixed face and bend faces" - turns on the face selection mode in the drawing.

3D History

CAD software 3D Module 850"Unbend". As part of the CAD drawing 3D Module 851 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drafting 3D Module 852.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Bend

Important!

This functionality requires a C3D 3D modeling engine.

CAD software 3D Module 853Main menu: 3D - Sheet metal - CAD drawing 3D Module 854Bend.

CAD drafting 3D Module 855Ribbon: 3D Tools - Sheet solids - CAD software 3D Module 856Bend.

CAD drawing 3D Module 857Toolbar: Sheet metal - CAD drafting 3D Module 858Bend.

CAD software 3D Module 859Command line: SMBEND.

The command allows you to bend previously unfolded sections of a sheet body.

Procedure

1. Call command CAD drawing 3D Module 860"Bend". The "Bend" dialog will open.

CAD drafting 3D Module 861

2. Select the main face to bend in the plane and the adjacent face (bend). Red cursorCAD software 3D Module 862 means selection mode is on. If no faces are selected, the corresponding red "Fixed face and faces for bending are not selected" text is displayed.

CAD drawing 3D Module 863CAD drafting 3D Module 864

If you need to replace a face or add faces, re-enter selection mode by pressing the CAD software 3D Module 865"Fixed face and faces for bending" button. To confirm your choice, click on CAD drawing 3D Module 866.

CAD drafting 3D Module 867CAD software 3D Module 868

3. Confirm the action with the "OK" button. The sheet solid will be bent. If the "OK" button is grayed out, then no faces were selected. A CAD drawing 3D Module 869"Bend" object will be created in the "3d History", with a snap to an existing or new body.

CAD drafting 3D Module 870

Button CAD software 3D Module 871"Fixed face and faces for bending" - turns on the face selection mode in the drawing.

3D History

CAD drawing 3D Module 872"Bend". As part of the CAD drafting 3D Module 873 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD software 3D Module 874.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Flatten

Important!

This functionality requires a C3D 3D modeling engine.

CAD drawing 3D Module 875Main menu: 3D - Sheet metal - CAD drafting 3D Module 876Flatten.

CAD software 3D Module 877Ribbon: 3D Tools - Sheet solids - CAD drawing 3D Module 878Flatten.

CAD drafting 3D Module 879Toolbar: Sheet metal - CAD software 3D Module 880Flatten.

CAD drawing 3D Module 881Command line: SMFLATTEN.

The command allows you to create a flat pattern of a sheet body.

Procedure

1. Call command CAD drafting 3D Module 882"Flatten". The "Flatten" dialog will open.

CAD software 3D Module 883

2. Select the face to unfold relative to. Red cursor CAD drawing 3D Module 884 means selection mode is on. If no face is selected, the corresponding red text "Fixed face is not selected" is displayed.

CAD drafting 3D Module 885

If you need to replace a face, re-enter selection mode by pressing the CAD software 3D Module 886"Fixed face" button.

3. Confirm the action with the "OK" button. The flatten will be built. If the "OK" button is grayed out, then no face has been selected. In the "3d History" object CAD drawing 3D Module 887"Flatten" will be created, with reference to an existing or new body.

CAD drafting 3D Module 888

Dialog

CAD software 3D Module 889

Button CAD drawing 3D Module 890"Fixed face" - turns on the face selection mode in the drawing.

Switch "Unbended" - controls the sweep state.

Switch "As a separate body" - creates a separate body.

3D History

CAD drafting 3D Module 891"Flatten". As part of the CAD software 3D Module 892 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drawing 3D Module 893.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Stamp

Important!

 

This functionality requires a C3D 3D modeling engine.

CAD drafting 3D Module 894Main menu: 3D - Sheet metal - CAD software 3D Module 895Stamp.

CAD drawing 3D Module 896Ribbon: 3D Tools - Sheet solids - CAD drafting 3D Module 897Stamp.

CAD software 3D Module 898Toolbar: Sheet metal - CAD drawing 3D Module 899Stamp.

CAD drafting 3D Module 900Command line: SMSTAMP.

Procedure

1. Draw a closed sketch on the face of the sheet body.

CAD software 3D Module 901

2. Call command CAD drawing 3D Module 902"Stamp". The "Stamp" dialog will open.

CAD drafting 3D Module 903

3. Select a sketch. A red cursor CAD software 3D Module 904 means that the sketch selection mode is on. If a sketch is not selected, the corresponding red "Sketch is not selected" is displayed.

CAD drawing 3D Module 905

If you need to replace the sketch (select another), re-enter the sketch selection mode by clicking the CAD drafting 3D Module 906"Sketch" button.

4. Specify the required parameters.

5. Confirm the action with the "OK" button. The stamp will be created. If the "OK" button is grayed out, it means that the sketch was not selected or the parameters were set incorrectly. In "3d History", a CAD software 3D Module 907"Stamp" object containing the sketch will be created and snapped to an existing or new solid.

CAD drawing 3D Module 908

Dialog

CAD drafting 3D Module 909

3D History

CAD software 3D Module 910"Stamp". As part of the CAD drawing 3D Module 911body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drafting 3D Module 912.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Jalousie

Important!

This functionality requires a C3D 3D modeling engine.

CAD software 3D Module 913Main menu: 3D - Sheet metal - CAD drawing 3D Module 914Jalousie.

CAD drafting 3D Module 915Ribbon: 3D Tools - Sheet solids - CAD software 3D Module 916Jalousie.

CAD drawing 3D Module 917Toolbar: Sheet metal - CAD drafting 3D Module 918Jalousie.

CAD software 3D Module 919Command line: SMJALOUSIE.

Procedure

1. Sketch on the face of the sheet body. Lines are used as sketches for the punch. The sketch must be completely within the base face of the feature.

CAD drawing 3D Module 920

2. Call command CAD drafting 3D Module 921"Jalousie". The "Jalousie" dialog will open.

CAD software 3D Module 922

3. Select a sketch. A red cursor CAD drawing 3D Module 923 means that the sketch selection mode is on. If a sketch is not selected, the corresponding red "Sketch is not selected" is displayed.

CAD drafting 3D Module 924

If you need to replace the sketch (select another), re-enter the sketch selection mode by clicking the CAD software 3D Module 925"Sketch" button.

4. Specify the required parameters.

5. Confirm the action with the "OK" button. The punch will be created. If the "OK" button is grayed out, it means that the sketch was not selected or the parameters were set incorrectly. If the preview does not show the punch, then the parameters are incorrect. In "3d History", a CAD drawing 3D Module 926"Jalousie" object containing a sketch is created and snapped to an existing or new solid.

CAD drafting 3D Module 927

Dialog

CAD software 3D Module 928

3D History

CAD drawing 3D Module 929"Jalousie". As part of the CAD drafting 3D Module 930 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD software 3D Module 931.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Bead

Important!

This functionality requires a C3D 3D modeling engine.

CAD drawing 3D Module 932Main menu: 3D - Sheet metal - CAD drafting 3D Module 933Bead.

CAD software 3D Module 934Ribbon: 3D Tools - Sheet solids - CAD drawing 3D Module 935Bead.

CAD drafting 3D Module 936Toolbar: Sheet metal - CAD software 3D Module 937Bead.

CAD drawing 3D Module 938Command line: SMBEAD.

Procedure

1. Sketch on the face of the sheet body. A sketch can contain multiple primitives.

CAD drafting 3D Module 939

2. Call command CAD software 3D Module 940"Bead". The "Bead" dialog will open.

CAD drawing 3D Module 941

3. Select a sketch. A red cursorCAD drafting 3D Module 942 means that the sketch selection mode is on. If a sketch is not selected, the corresponding red "Sketch is not selected" is displayed.

CAD software 3D Module 943

If you need to replace the sketch (select another), re-enter the sketch selection mode by clicking the CAD drawing 3D Module 944"Sketch" button.

4. Specify the required parameters.

5. Confirm the action with the "OK" button. The bend will be created. If the "OK" button is grayed out, it means that the sketch was not selected or the parameters were set incorrectly. In "3d History", a CAD drafting 3D Module 945"Bead" object containing a sketch will be created and referenced to an existing or new solid.

CAD software 3D Module 946

Dialog

CAD drawing 3D Module 947

3D History

CAD drafting 3D Module 948"Bead". As part of the CAD software 3D Module 949body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drawing 3D Module 950.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Rib

Important!

This functionality requires a C3D 3D modeling engine.

CAD drafting 3D Module 951Main menu: 3D - Sheet metal - CAD software 3D Module 952Rib.

CAD drawing 3D Module 953Ribbon: 3D Tools - Sheet solids - CAD drafting 3D Module 954Rib.

CAD software 3D Module 955Toolbar: Sheet metal - CAD drawing 3D Module 956Rib.

CAD drafting 3D Module 957Command line: SMRIB.

Procedure

1. Call command CAD software 3D Module 958"Rib". The "Rib" dialog will open.

CAD drawing 3D Module 959

2. Select an edge at the bend location. Red cursor CAD drafting 3D Module 960 means selection mode is on. If the edge is not selected, the corresponding red text "Bending edge is not selected" is displayed.

CAD software 3D Module 961CAD drawing 3D Module 962

If you need to replace an edge (select another), enter the selection mode again by pressing the CAD drafting 3D Module 963"Bending edge" button.

3. Specify the required parameters.

4. Confirm the action with the "OK" button. The rib will be built. If the "OK" button is inactive, it means that the object was not selected or the parameters were set incorrectly. In the "3d History" object CAD software 3D Module 964"Rib" will be created, with a connection to an existing or new body.

CAD drawing 3D Module 965

Dialog

CAD drafting 3D Module 966

3D History

CAD software 3D Module 967"Rib". As part of the CAD drawing 3D Module 968 body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drafting 3D Module 969.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Flanging

Important!

This functionality requires a C3D 3D modeling engine.

CAD software 3D Module 970Main menu: 3D - Sheet metal - CAD drawing 3D Module 971Flanging.

CAD drafting 3D Module 972Ribbon: 3D Tools - Sheet solids - CAD software 3D Module 973Flanging.

CAD drawing 3D Module 974Toolbar: Sheet metal - CAD drafting 3D Module 975Flanging.

CAD software 3D Module 976Command line: SMFLANGING.

Procedure

1. Call command CAD drawing 3D Module 977"Flanging". The "Flanging" dialog will open.

2. Select the edges on the sheet body. The red cursor CAD drafting 3D Module 978 means that the selection mode is enabled. If an edge is not selected, the corresponding red caption "Not selected: Edges" is displayed.

CAD software 3D Module 979CAD drawing 3D Module 980

Select the required number of ribs. To cancel the selection, reselect the edge.

CAD drafting 3D Module 981

To complete the selection, select the "Finish" context menu command. If you need to replace the edge (select another one), enter the selection mode again by pressing the CAD software 3D Module 982"Ribs" button.

3. Specify the required parameters on the form.

5. Confirm the action on the "OK" button. The flanging will be built. If the "OK" button is inactive, it means that the object was not selected or the parameters were set incorrectly. In the "3D History" the CAD drawing 3D Module 983"Flanging" object will be created, with reference to an existing or new part.

Dialog

3D History

CAD drafting 3D Module 984"Flanging". As part of the CAD software 3D Module 985body.

The following context menu commands are available:

     ·     Edit - calls the object for editing. The edit symbol appears to the right of the icon CAD drawing 3D Module 986.

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from tree and model space.

     ·     Suppress - removes an object from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Editing

3D Align

CAD drafting 3D Module 987Main menu: 3D -3D Features - CAD software 3D Module 9883D Align.

CAD drawing 3D Module 989Ribbon: 3D Tools - Solid Editing - CAD drafting 3D Module 9903D Align.

CAD software 3D Module 991Toolbar: 3D - CAD drawing 3D Module 9923D Align.

CAD drafting 3D Module 993Command line: 3DALIGN.

A tool for pairing surfaces, curves, or points in model space.

Note:

Information about the alignment does not fall into the "3DHistory".

Procedure

1. Call command CAD software 3D Module 994"3D Align".

2. Specify the objects that you want to align. To complete the selection, press the "Enter" key. The dialog "3D Align" will open.

CAD drawing 3D Module 995

3. Use the "3D Align" dialog to select the locations in one of three ways:

     ·     Surface to Surface. The surface can be a face of a part or a plane. In this method, the surface is adjacent to the surface. When using the button CAD drafting 3D Module 996"Change Direction" the direction of aligned objects is changing.

CAD software 3D Module 997CAD drawing 3D Module 998

     ·     Curve to Curve. The axis can be an edge of the part or an axis. In this method, the selected axes are combined. When using the button CAD drafting 3D Module 999"Change Direction" the direction of aligned objects is changing.

CAD software 3D Module 1000CAD drawing 3D Module 1001

     ·     Point to point. In this method, points are combined.

CAD drafting 3D Module 1002CAD software 3D Module 1003

4. When all the locations have been selected, click "OK". Alignment will be performed.

Manipulators

Manipulators allow you to manipulate the 3D model: move, rotate or change the scale.

There are two ways to use manipulators:

1. Force a call using the appropriate commands: 3D Move, 3D Rotate, 3D Scale.

2. Automatic call of the configured manipulator when selecting a 3D model (the call does not work in 2D Wireframe mode).

Setting up automatic call

The DEFAULTMANIPULATOR system variable (default keyer) is responsible for configuring the automatic call of the manipulator.

Manipulators and how to install them:

1. Move Manipulator

CAD drawing 3D Module 1004Main menu: 3D - 3D Features - CAD drafting 3D Module 1005Move Manipulator.

CAD software 3D Module 1006Ribbon: 3D Tools - Manipulators - CAD drawing 3D Module 10073D Move Manipulator.

CAD drafting 3D Module 1008Toolbar: 3D Transformations - CAD software 3D Module 1009Move Manipulator.

CAD drawing 3D Module 1010Command line: DEFAULTMANUPULATOR1.

CAD drafting 3D Module 1011Command line: DEFAULTMANUPULATOR - set to 1 or select "Move manipulator".

2. Rotate Manipulator

CAD software 3D Module 1012Main menu: 3D -3D Features - CAD drawing 3D Module 1013Rotate Manipulator.

CAD drafting 3D Module 1014Ribbon: 3D Tools - Manipulators - CAD software 3D Module 10153D Rotate Manipulator.

CAD drawing 3D Module 1016Toolbar: 3D Transformations - CAD drafting 3D Module 1017Rotate Manipulator.

CAD software 3D Module 1018Command line: DEFAULTMANUPULATOR2.

CAD drawing 3D Module 1019Command line: DEFAULTMANUPULATOR - set to 2 or select "Rotate manipulator".

3. Scale Manipulator

CAD drafting 3D Module 1020Main menu: 3D -3D Features - CAD software 3D Module 1021Scale Manipulator.

CAD drawing 3D Module 1022Ribbon: 3D Tools - Manipulators - CAD drafting 3D Module 10233D Scale Manipulator.

CAD software 3D Module 1024Toolbar: 3D Transformations - CAD drawing 3D Module 1025Scale Manipulator.

CAD drafting 3D Module 1026Command line: DEFAULTMANUPULATOR3.

CAD software 3D Module 1027Command line: DEFAULTMANUPULATOR - set to 3 or select "Scale manipulator".

4. No Manipulator

CAD drawing 3D Module 1028Main menu: 3D - 3D Features - CAD drafting 3D Module 1029No Manipulator.

CAD software 3D Module 1030Ribbon: 3D Tools - Manipulators - CAD drawing 3D Module 1031Without Manipulator.

CAD drafting 3D Module 1032Toolbar: 3D Transformations - CAD software 3D Module 1033No Manipulator.

CAD drawing 3D Module 1034Command line: DEFAULTMANUPULATOR4.

CAD drafting 3D Module 1035Command line: DEFAULTMANUPULATOR - set to 4 or select "No manipulator".

3D Move

CAD software 3D Module 1036Main menu: 3D - 3D Features - CAD drawing 3D Module 10373D Move.

CAD drafting 3D Module 1038Ribbon: 3D Tools - Solid Editing - CAD software 3D Module 10393D Move.

CAD drawing 3D Module 1040Toolbar: 3D - CAD drafting 3D Module 10413D Move.

CAD software 3D Module 1042Toolbar: 3D Transform - CAD drawing 3D Module 10433D Move.

CAD drafting 3D Module 1044Command line: 3DMOVE.

Tool for moving part in model space.

Important!

Without the 3D module for "Nonparametric solid" objects, the manipulator works in demo mode, i.e. there will be no actual movement.

Procedure

1. Call command CAD software 3D Module 1045"3D Move".

2. Select part in model space or in "3D History". The sketch part should not be tied to one of the main planes of the model. The selected parts are highlighted in green, and the selected ones in yellow. You can select multiple parts in one operation. After completing the selection, press the "Enter" key or the "Enter" command from the context menu.

CAD drawing 3D Module 1046

3. Select the axis or plane along which the movement will occur.

CAD drafting 3D Module 1047

4. Forward movements of the mouse move part along the selected axis (plane). You can also enter the value of the navigation from the keyboard.

CAD software 3D Module 1048

5. Repeat the movement as many times as necessary (p.3-p.4). When the transfer is complete, press the "Enter" key or the "Enter" command from the context menu.

3D Rotate

CAD drawing 3D Module 1049Main menu: 3D - 3D Features - CAD drafting 3D Module 10503D Rotate.

CAD software 3D Module 1051Ribbon: 3D Tools - Solid Editing - CAD drawing 3D Module 10523D Rotate.

CAD drafting 3D Module 1053Toolbar: 3D - CAD software 3D Module 10543D Rotate.

CAD drawing 3D Module 1055Toolbar: 3D Transform - CAD drafting 3D Module 10563D Rotate.

CAD software 3D Module 1057Command line: 3DROTATE.

Tool for rotating part in model space.

Important!

Without the 3D module for "Nonparametric solid" objects, the manipulator works in demo mode, i.e. there will be no actual movement.

Procedure

1. Call command CAD drawing 3D Module 1058"3D Rotate".

2. Select the rotating part in the model space or in the "3D History". The sketch part should not be tied to one of the main planes of the model. The selected parts are highlighted in green, and the selected ones in yellow. You can select multiple parts in one operation. When the selection is complete, press the "Enter" key or the "Enter" command from the context menu.

CAD drafting 3D Module 1059

3. Select the base point on the rotated part. This point will be the center of rotation around the selected axis.

CAD software 3D Module 1060

4. Select the axis along which the rotation will occur.

CAD drawing 3D Module 1061

5. In the forward movements of the mouse, rotate the part along the selected axis. You can also enter the value of the rotation angle from the keyboard.

CAD drafting 3D Module 1062

6. Repeat the rotation as many times as necessary (p.3-p.5). When the transfer is complete, press the "Enter" key or the "Enter" command from the context menu.

3D Scale

CAD software 3D Module 1063Main menu: 3D - 3D Features - CAD drawing 3D Module 10643D Scale.

CAD drafting 3D Module 1065Ribbon: 3D Tools - Solid Editing - CAD software 3D Module 10663D Scale.

CAD drawing 3D Module 1067Toolbar: 3D - CAD drafting 3D Module 10683D Scale.

CAD software 3D Module 1069Toolbar: 3D Transform - CAD drawing 3D Module 10703D Scale.

CAD drafting 3D Module 1071Command line: 3DSCALE.

3D scaling allows you to resize selected objects and subobjects along an axis or a plane or to scale objects uniformly.

Important!

The command applies only to objects "3D Solid" and "Polyface Mesh"

 

Important!

Without the 3D module for "Nonparametric solid" objects, the manipulator works in demo mode, i.e. there will be no actual movement.

Procedure

1. Call command CAD software 3D Module 1072"3D Scale";

2. Select objects that require scaling;

CAD drawing 3D Module 1073

3. Press the key "Enter (Space)";

4. Specify the base point of scaling;

CAD drafting 3D Module 1074

5. Specify a scale axis or a scale plane;

     ·     Same scale. Click the area near the top of the 3D Scaling. The internal part of all axes stands out. Scaling will be performed evenly across all three axes.

CAD software 3D Module 1075

     ·     Limitation of scaling by the position of the plane. Click between the parallel lines located between the axes defining the plane. Scaling will be done in two axes. This operation is only for Mesh, it is not applicable to 3D Solid and surfaces.

CAD drawing 3D Module 1076

     ·     Scale limiting by axis position. Click the Axis. Scaling will be done on one axis. This operation is only for Mesh, it is not applicable to 3D Solid and surfaces

CAD drafting 3D Module 1077

6. Set the scale (on the drawing or on the command line), objects will be scaled;

CAD software 3D Module 1078

7. Repeat steps 4-6 as many times as necessary. To end the command, press  "Esc (Space)".

3D Rectangular Array

CAD drawing 3D Module 1079Main menu: 3D - 3D Features - CAD drafting 3D Module 10803D Rectangular Pattern.

CAD software 3D Module 1081Ribbon: 3D Tools - Solid Editing - CAD drawing 3D Module 10823D Rectangular Array.

CAD drafting 3D Module 1083Toolbar: 3D - CAD software 3D Module 10843D Rectangular Pattern.

CAD drawing 3D Module 1085Command line: 3DRECTPAT.

Tool for creating an array in one or two directions.

Procedure

1. Call command CAD drafting 3D Module 1086"3D Rectangular Pattern". Open dialog "3D Rectangular Pattern".

CAD software 3D Module 1087

2. Select the type of objects involved in the creation of the array:

     ·     CAD drawing 3D Module 1088Array of features. An array of elements will refer to the original body.

CAD drafting 3D Module 1089

Note:

Chamfers and fillets can not be received by the array as separate elements; You can not make an array of chamfers or fillets!

Chamfers and fillets can be used only as a part of bodies.

     ·     CAD software 3D Module 1090Array of bodies. The whole body goes to the array, a new body with an element will be created CAD drawing 3D Module 1091"McRectangularPatternFeature".

CAD drafting 3D Module 1092

3. Select elements to create an array.

4. Adjust the array parameters, or take them from the sample array.

Parameters from sample array:

     ·     Press button CAD software 3D Module 1093"Get parameters from sample array".

     ·     Specify sample array.

     ·     The created array will be passed: direction, quantity, distance and type of distance.

Specifying parameters yourself:

     ·     Select the first direction of the array. The axis of the GCS, the working axis or the edge of any body can be used as a direction. The phantom of the created array is highlighted in orange.

     ·     Invert if necessary the direction of the layout of elements with the button CAD drawing 3D Module 1094"Flip direction".

     ·     Specify the number of copies in the input field CAD drafting 3D Module 1095"Count elements".

     ·     Enter the distance in the input field CAD software 3D Module 1096"Distance". To the right of the input field is a button CAD drawing 3D Module 1097"Measure distance", allowing you to take a value from the drawing.

     ·     Select distance type:

                 ·     Filling step - sets the distance between each element in the array.

                 ·     Filling range - sets the distance between the extreme elements in the array.

     ·     Repeat steps for the second direction, if the array is built in two directions.

5. Press button "OK". An array will be created based on the selected items. In the "3D History" an object appears CAD drafting 3D Module 1098"McRectangularPatternFeature".

3D History

CAD software 3D Module 1099"McRectangularPatternFeature". It is part of the body. When creating an array from the elements of the source body, the object CAD drawing 3D Module 1100"McRectangularPatternFeature" falls into the composition of the original body. When creating an array from the source body, a new body is created, object CAD drafting 3D Module 1101"McRectangularPatternFeature" falls into the new body.

The object CAD software 3D Module 1102"McRectangularPatternFeature" includes: folder CAD drawing 3D Module 1103"Elements" with a list of source elements or folder CAD drafting 3D Module 1104"Solids" with a list of source bodies, and links CAD software 3D Module 1105"Occurrence", showing the elements of the array in model space.

The following commands of the object's context menu are available  CAD drawing 3D Module 1106"McRectangularPatternFeature":

     ·     Edit - opens the editing dialog  "3D Rectangular Pattern".

     ·     Rename (F2) - allows you to rename a pattern.

     ·     Delete (Del) - removes a pattern from the tree and model space.

     ·     Suppress - removes a pattern from model space.

     ·     Unsupress - restores a pattern in model space.

     ·     ShowInDocument - focuses and highlights a pattern in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

3D Polar Array

CAD drafting 3D Module 1107Main menu: 3D - 3D Features - CAD software 3D Module 11083D Circular Pattern.

CAD drawing 3D Module 1109Ribbon: 3D Tools - Solid Editing - CAD drafting 3D Module 11103D Polar Array.

CAD software 3D Module 1111Toolbar: 3D - CAD drawing 3D Module 11123D Circular Pattern.

CAD drafting 3D Module 1113Command line: 3DCIRCPAT.

Tool for creating an array of elements or bodies around a certain axis.

Procedure

1. Call command CAD software 3D Module 1114"3D Circular Pattern". Open dialog "3D Circular Pattern".

CAD drawing 3D Module 1115

2. Select the type of objects involved in the creation of the array:

     ·     CAD drafting 3D Module 1116Array of features. An array of elements will refer to the original part.

CAD software 3D Module 1117

Note:

Chamfers and fillets can not be received by the array as separate elements; You can not make an array of chamfers or fillets!

Chamfers and fillets can be used only as a part of bodies.

     ·     CAD drawing 3D Module 1118Array of bodies. he whole body goes to the array, a new body with an element will be created CAD drafting 3D Module 1119"McCircularPatternFeature".

CAD software 3D Module 1120

3. Select elements to create an array.

4. Adjust the array parameters, or take them from the sample array.

Parameters from sample array:

     ·     Press button CAD drawing 3D Module 1121"Get parameters from sample array".

     ·     Specify sample array.

     ·     The following will be passed to the created array: axis of rotation, direction, amount, angle and type of filling.

Specifying parameters yourself:

     ·     Select the axis. As an axis, the GCS axis, the working axis or the edge of any body can be used. Orange color is highlighted by a phantom of the created array.

Important!

The edges of the bodies involved in the creation of the array cannot be used as an axis. It turns out that one edge participates in several closed shells, and the parts to be combined can never exactly touch each other. Existing 3D kernels process this data incorrectly, so such an array is likely to be built erroneously.

In order to correct, you can use the auxiliary axis, slightly shifted in parallel from the desired one, for example, by 1 μm.

     ·     Invert if necessary the direction of the layout of elements with the button CAD drafting 3D Module 1122"Flip direction". By default, the layout is clockwise.

     ·     Enter the number of copies in the input field CAD software 3D Module 1123"Count of items".

     ·     Specify the angle in the input field CAD drawing 3D Module 1124"Angle for items". To the right of the input field is the button CAD drafting 3D Module 1125"Measure angle", allowing you to take a value from the drawing.

     ·     Specify the type of filling:

                 ·     Filling angle - sets the value of the fill angle between the extreme elements in the array.

                 ·     Spacing angle - sets the value of the step between each element in the array.

5. Press button "OK". An array will be created based on the selected elements. In the "3D History" object appears CAD software 3D Module 1126"McCircularPatternFeature".

3D History

CAD drawing 3D Module 1127"McCircularPatternFeature".It is part of the part. When creating an array from the elements of the source body, the object CAD drafting 3D Module 1128"McCircularPatternFeature" falls into the composition of the original body. When creating an array from the source body, a new body, object CAD software 3D Module 1129"McCircularPatternFeature" falls into the new body.

The objectCAD drawing 3D Module 1130"McCircularPatternFeature" includes: folder CAD drafting 3D Module 1131"Elements" with a list of source elements or folder CAD software 3D Module 1132"Solids" with a list of source bodies, and links CAD drawing 3D Module 1133"Occurrence", showing array elements in the model space.

The following commands of the object's context menu are available  CAD drafting 3D Module 1134"McCircularPatternFeature":

     ·     Edit - opens the editing dialog  "3D Circular Pattern".

     ·     Rename (F2) - allows you to rename an array.

     ·     Delete (Del) - removes an array from the tree and model space.

     ·     Suppress - removes an array from model space.

     ·     unsuppress - restores an array in model space.

     ·     ShowInDocument - focuses and highlights the array in the center of the model space.

     ·     Rebulid - rebuilds the object in model space.

3D Fillet

CAD software 3D Module 1135Main menu: 3D - 3D Features - CAD drawing 3D Module 11363D Fillet.

CAD drafting 3D Module 1137Ribbon: 3D Tools - Solid Editing - CAD software 3D Module 1138Fillet Edge.

CAD drawing 3D Module 1139Toolbar: 3D - CAD drafting 3D Module 11403D Fillet.

CAD software 3D Module 1141Command line: 3DFILLET.

Tool for creating different kinds of fillets.

Procedure

1. Call command CAD drawing 3D Module 1142"3D Fillet". The "3D Fillet" dialog will be opened.

CAD drafting 3D Module 1143

2. Define the rib selection method using the "Edge chain".

CAD software 3D Module 1144 - the edges are selected one at a time

CAD drawing 3D Module 1145 - select all edges of the selected face

CAD drafting 3D Module 1146

CAD software 3D Module 1147

3. Select the edges. During the selection process, the rounding phantoms will be visible in the modeling environment.

4. Specify the radius. To the right of the radius input field is the button CAD drawing 3D Module 1148"Measure radius", allowing to take the value from the drawing.

5. Press the "OK" key. Fillets will be built. In the "3D History" in the part will be an object CAD drafting 3D Module 1149"McFilletFeature".

3D History

CAD software 3D Module 1150"McFilletFeature". It is found in the part.

The following shortcut menu commands are available:

     ·     Edit - opens the editing dialog "3D Fillet".

     ·     Rename (F2) - allows you to rename a fillet.

     ·     Delete (Del) - removes fillet from tree and model space.

     ·     Suppress - removes fillet from model space.

     ·     Unsuppress - restores the fillet in the model space.

     ·     ShowInDocument - focuses and highlights the fillet at the center of the model space.

     ·     Rebuild - rebuilds an object in model space.

3D Chamfer

CAD drawing 3D Module 1151Main menu: 3D - 3D Features - CAD drafting 3D Module 11523D Chamfer.

CAD software 3D Module 1153Ribbon: 3D Tools - Solid Editing - CAD drawing 3D Module 1154Chamfer Edge.

CAD drafting 3D Module 1155Toolbar: 3D - CAD software 3D Module 11563D Chamfer.

CAD drawing 3D Module 1157Command line: 3DCHAMFER.

Tool for creating all kinds of chamfers.

Procedure

1. Call command CAD drafting 3D Module 1158"3D Chamfer". Open dialog "3D Chamfer".

Note:

Simultaneously, on two or more bodies the facet can not be built. You need to call the CAD software 3D Module 1159"3D Chamfer" command for each body separately.

2. In the "3D Chamfer" dialog, select the method for creating the chamfer and specify the required parameters, depending on the method:

     ·     CAD drawing 3D Module 1160Equal distances from both faces - it makes it possible to build a chamfer in one dimension - length. The angle is automatically equal to 45°.

CAD drafting 3D Module 1161

                 ·     Define the rib selection method using the "Edge chain".

CAD software 3D Module 1162 - the edges are selected one at a time

CAD drawing 3D Module 1163 -select all edges of the selected face

CAD drafting 3D Module 1164

CAD software 3D Module 1165

                 ·     Select the edges. During the selection process, the chamfering phantoms will be visible in the simulation environment.

                 ·     Enter the distance. To the right of the distance input field is the button CAD drawing 3D Module 1166"Measure distance", allowing to take the value from the drawing.

CAD drafting 3D Module 1167

     ·     CAD software 3D Module 1168Distance and angle from specify face - it is possible to construct a facet by the angle and length of the selected face.

CAD drawing 3D Module 1169

                 ·     Select face.

                 ·     Determine the method for selecting edges using the switch group "Edge chain".

                 ·     Select the edges of this face. During the selection process, the chamfering phantoms will be visible in the modeling environment.

                 ·     Enter the distance. To the right of the distance input field is the button CAD drafting 3D Module 1170"Measure distance", allowing to take the value from the drawing.

                 ·     Enter the angle. To the right of the distance input field is the button CAD software 3D Module 1171"Measure angle", allowing to take the value from the drawing.

CAD drawing 3D Module 1172

     ·     CAD drafting 3D Module 1173Two distances -it is possible to construct a facet on two distances from the edge.

CAD software 3D Module 1174

                 ·     Determine the method for selecting edges using the switch group "Edge chain".

                 ·     Select the edges. During the selection process, the chamfering phantoms will be visible in the modeling environment.

                 ·     Enter the distances. To the right of the distance input fields are the buttons CAD drawing 3D Module 1175"Measure distance", allowing to take the value from the drawing.

                 ·     If necessary, invert the distance values using the button CAD drafting 3D Module 1176"Invert values".

CAD software 3D Module 1177

3. Press button "OK". Chamfers will be built. In the "3D History" in the part will be an object CAD drawing 3D Module 1178"McChamferFeature".

3D History

CAD drafting 3D Module 1179"McChamferFeature".It is found in the part.

The following shortcut menu commands are available:

     ·     Edit - opens the editing dialog  "3D Chamfer".

     ·     Rename (F2) - allows you to rename a chamfer.

     ·     Delete (Del) - removes the chamfer from the tree and model space.

     ·     Suppress - removes a chamfer from the model space.

     ·     Unsuppress - restores a chamfer in model space.

     ·     ShowInDocument - focuses and highlights the chamfer in the center of the model space.

     ·     Rebuild - rebuilds an object in model space.

3D Thread

CAD software 3D Module 1180Main menu: 3D - 3D Features - CAD drawing 3D Module 11813D Thread.

CAD drafting 3D Module 1182Ribbon: 3D Tools - Details - CAD software 3D Module 1183Thread.

CAD drawing 3D Module 1184Toolbar: 3D - CAD drafting 3D Module 11853D Thread.

CAD software 3D Module 1186Command line: 3DTHREAD.

The command sets the thread on the selected cylindrical section of the 3D body.

Procedure

CAD drawing 3D Module 1187

1. Call command "3D Thread". The "3D Thread" dialog will open. When the command is running, the visual style will be set to "Fast shaded".

CAD drafting 3D Module 1188

2. Specify "Thread face". The face should be cylindrical.

CAD software 3D Module 1189

3. Make thread settings in the "3D Thread" dialog and click the "OK" button.

CAD drawing 3D Module 1190

4. The thread will be built. The visual style will revert to the original. In "3D History", a "Thread" object is added to the body.

CAD drafting 3D Module 1191

Edit

Called in the "3D History" from the context menu of the "Thread" object.

CAD software 3D Module 1192

The editing dialog is divided into parts:

     ·     Face selection panel

CAD drawing 3D Module 1193

Button "Thread face" - allows you to select a cylindrical face to thread onto.

Button "Front edge" - allows you to select the thread origin face.

     ·     Standart

CAD drafting 3D Module 1194

Combobox "Standart" - allows you to select the thread standard.

     ·     Thread Parameter Panel

CAD software 3D Module 1195

Combobox "Pitch" - allows you to select the thread pitch. The list of options depends on the diameter of the cylindrical face and the selected standard.

Field "External size" - shows the outer diameter of the thread. The field is not editable.

Field "Internal size" - shows the inside diameter of the thread. The field is not editable.

Field "Designation" - shows the thread designation. The input field is not editable.

     ·     Panel for setting thread length and direction

CAD drawing 3D Module 1196

Checkbox "Full length" - controls the setting of the thread length. If the switch is on - the length of the thread is determined by the length of the cylindrical face, off - the length of the thread is specified in the "Depth" input field.

Field "Depth" - specifies the thread length.

Group switch for thread direction - "Right" or "Left".

     ·     Dashboard

CAD drafting 3D Module 1197

Shows errors and remarks when setting up threads.

3D History

CAD software 3D Module 1198"Thread". As part of the CAD drawing 3D Module 1199body.

The following context menu commands are available:

     ·      Edit - the command opens the thread editing dialog "3D Thread".

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes object and child objects from tree and model space.

     ·     Suppress - removes object and child objects from model space.

     ·     Unsuppress - restores the object in model space.

     ·     ShowInDocument - focuses and highlights the subject in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

3D Mirrow

CAD drafting 3D Module 1200Main menu: 3D - 3D Features - CAD software 3D Module 12013D Mirror.

CAD drawing 3D Module 1202Ribbon: 3D Tools - Solid Editing - CAD drafting 3D Module 12033D Mirror.

CAD software 3D Module 1204Toolbar: 3D - CAD drawing 3D Module 12053D Mirror.

CAD drafting 3D Module 1206Command line: 3DMIRROR.

Tool for creating a reflection of an element or a body with respect to the plane of reflection. The command works only with parametric solids.

Procedure

1. Call command CAD software 3D Module 1207"3D Mirror". Open dialog "3D Mirror".

CAD drawing 3D Module 1208

2. In the "3D Mirror" dialog, select the type of reflection:

     ·     CAD drafting 3D Module 1209Array of features. Reflected body elements and reflection will refer to the original body.

CAD software 3D Module 1210

     ·     CAD drawing 3D Module 1211Array of bodies. The whole body is reflected, a new body with an element will be created  CAD drafting 3D Module 1212"McMirrorFeature".

CAD software 3D Module 1213

3. Select elements or body, depending on the type of reflection selected.

4. Select the reflection plane. It can be the plane of the coordinate system, the working plane or the face of any body. When selecting a reflection plane, a phantom reflective appears.

5.Press button "OK". Reflection will be created based on the selected items. In the "3D History" an object appears CAD drawing 3D Module 1214"McMirrorFeature".

3D History

CAD drafting 3D Module 1215"McMirrorFeature". It is part of the body. When the elements of the original body are reflected, the object CAD software 3D Module 1216"McMirrorFeature" falls into the composition of the original body. When the original body is reflected, a new body, object CAD drawing 3D Module 1217"McMirrorFeature" falls into the new body.

The object CAD drafting 3D Module 1218"McMirrorFeature" includes: folder CAD software 3D Module 1219"Elements" with a list of source elements or folder CAD drawing 3D Module 1220"Solids" with a list of source bodies, and two links CAD drafting 3D Module 1221"Occurrence",showing in the model space the finding of the original elements and reflected.

The following commands of the object's context menu are available  CAD software 3D Module 1222"McMirrorFeature":

     ·     Edit - opens the editing dialog  "3D Mirror".

     ·     Rename (F2) - allows you to rename an object.

     ·     Delete (Del) - removes an object from the tree and model space.

     ·     Suppress - removes the mirrored object from the model space.

     ·     Unsuppress - restores a mirrored object in model space.

     ·     ShowInDocument - focuses and highlights the mirrored object in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Union

CAD drawing 3D Module 1223Ribbon: 3D Tools - Solid Editing - CAD drafting 3D Module 1224Union.

CAD software 3D Module 1225Toolbar: 3D - CAD drawing 3D Module 1226Union.

CAD drafting 3D Module 1227Command line: UNION.

The tool allows you to combine parametric objects or 3D solidities.

Procedure

1. Call command CAD software 3D Module 1228"Union";

2. Specify the merge objects;

CAD drawing 3D Module 1229

3. Press the  "Enter (Space)" key;

4. Union will be made. All selected objects become one object. In "3D History", the first selected body will display an object CAD drafting 3D Module 1230"Union", containing all selected bodies except the first.

CAD software 3D Module 1231

Note:

If the objects were selected before the "Union" command is called, the union will be automatically generated immediately after the call.

3D History

CAD drawing 3D Module 1232"Union". It is part of the parent part, contains parts that are combined with the parent part.

The following shortcut menu commands are available:

     ·     Rename (F2) - allows you to rename an association.

     ·     Delete (Del) - removes the union and its associated objects from the tree and model space.

     ·     Suppress - suppresses the union. With the parts included in the union, you can treat as individual objects.

     ·     Unsupress - restores the union.

     ·     ShowInDocument - focuses and highlights the incoming bodies in the center of model space.

     ·     Rebuild - rebuilds an object in model space.

Intersect

CAD drafting 3D Module 1233Ribbon: 3D Tools - Solid Editing - CAD software 3D Module 1234Intersection.

CAD drawing 3D Module 1235Toolbar: 3D - CAD drafting 3D Module 1236Intersect.

CAD software 3D Module 1237Command line: INTERSECT.

The tool allows you to create an object based on the intersection of several objects. That is, the new object will be the joint intersected area.

Procedure

1. Call command CAD drawing 3D Module 1238"Intersect";

2. Specify intersecting objects;

CAD drafting 3D Module 1239

3. Press the  "Enter (Space)" key;

4. A new object based on the intersection will be created. In "3D History", the first selected body will display an object CAD software 3D Module 1240"Intersect", containing all selected bodies except the first.

CAD drawing 3D Module 1241

Note:

If the objects were selected before the "Intersect" command is called, the intersection will be automatically generated immediately after the call.

3D History

CAD drafting 3D Module 1242"Intersect". It is part of the parent part, contains parts that intersect with the parent part.

The following shortcut menu commands are available:

     ·     Rename (F2) - allows you to rename an intersection.

     ·     Delete (Del) - removes the intersection and associated objects from the tree and model space.

     ·     Suppress - suppresses the intersection action. With bodies entering the intersection, you can treat both as individual objects.

     ·     Unsuppress - restores the intersection action.

     ·     ShowInDocument - focuses and highlights the faces obtained as a result of the intersection, in the center of the model space.

     ·     Rebuild - rebuilds an object in model space.

Subtract

CAD software 3D Module 1243Ribbon: 3D Tools - Solid Editing - CAD drawing 3D Module 1244Subtraction.

CAD drafting 3D Module 1245Toolbar: 3D - CAD software 3D Module 1246Subtract.

CAD drawing 3D Module 1247Command line: SUBTRACT.

The tool allows you to create an object based on the selected objects by subtracting one of the others (the objects are divided into those from which the subtraction will be made and those that will subtract).

Procedure

1. Call command CAD drafting 3D Module 1248"Subtract";

2. Specify the objects from which the subtraction will be made;

CAD software 3D Module 1249

3. Specify the objects that will be subtracted;

CAD drawing 3D Module 1250

4. Press the  "Enter (Space)" key;

5. A new object will be created. If the number of bodies from which a subtraction of more than one was made, then in "3D History" in the first subtrahend body appears object CAD drafting 3D Module 1251"Subtract", containing all subtrahend bodies except the first. In the same body, an object will appear CAD software 3D Module 1252"Intersect", containing all subtractive bodies.

CAD drawing 3D Module 1253

Note:

If the objects from which the subtraction will be made were selected before the "Subtract" command is called, then the command immediately proceeds to the selection of subtracting objects.

3D History

CAD drafting 3D Module 1254"Subtract". It is part of the parent body, contains bodies that are subtracted from the parent.

The following shortcut menu commands are available:

     ·     Rename (F2) - allows you to rename subtraction.

     ·     Delete (Del) - removes subtraction and related objects from the tree and model space.

     ·     Suppress - suppresses the subtraction action. With the parts included in the subtraction, one can treat both as individual objects.

     ·     Unsuppress - restores the subtraction action.

     ·     ShowInDocument - focuses and highlights the edges obtained as a result of subtraction, in the center of the model space.

     ·     Rebuild - rebuilds an object in model space.

Add work plane

CAD software 3D Module 1255Main menu: 3D - 3D Features - CAD drawing 3D Module 1256Add work plane.

CAD drafting 3D Module 1257Ribbon: 3D Tools - Solid Editing - CAD software 3D Module 1258Add work plane.

CAD drawing 3D Module 1259Toolbar: 3D - CAD drafting 3D Module 1260Add work plane.

CAD software 3D Module 1261Command line: ADDWPL.

A tool that allows you to add a new plane to the model space.

Procedure

1. Call command CAD drawing 3D Module 1262"Add work plane".

2. Choose how to build a plane from the context menu or command line:

     ·     select object - the construction of a plane by choosing a face or a part edge.

     ·     3PT - plane construction by three points.

     ·     2LN - the construction of a plane along two axes (segments can also be axes for constructing a plane).

     ·     WPL_NORM2CURV - the construction of the plane is normal to the curve. To build, you must specify a curve and a point.

     ·     WPL_NORM2SURF - the construction of a plane normal to the surface. To build, you must specify a surface and a point.

     ·     LPANG - the construction of the plane along the axis, plane and angle. The angle is measured from the selected plane counterclockwise.

     ·     PLOFS - plot the plane at a distance from the selected one.

3. Select the required objects according to the chosen method of plotting the plane. To facilitate the selection of "the main coordinate system selection items", commands will be available in the context menu:

     ·     Origin - Selects the point of intersection of the main axes of coordinates.

     ·     X, Y, Z - Selects axes of the main coordinate system.

     ·     XY, YZ, ZX - Selects the planes of the main coordinate system.

4. The "Work Plane" object will be created and added to "3D History".

Properties

Does not have individual properties.

Grips

CAD drafting 3D Module 1263Moving grip - serves to move the plane in the model space. It is recommended not to use.

3D History

CAD software 3D Module 1264 Work plane. Can be located in the root of the tree and enter the structure of objects  CAD drawing 3D Module 1265"Part".

The following shortcut menu commands are available:

     ·     Rename (F2) - allows you to rename a plane.

     ·     Delete (Del) - removes the plane and related objects from the tree and model space.

     ·     Create 2d-sketch - calls the command "Add planar sketch". The drawing sketch plane is not necessary.

     ·     Hide - hides the mapping of the plane in model space.

     ·     Show - shows the mapping of the plane in model space.

     ·     Fix - fixes a plane in model space. An anchor label is added to the plane icon. The command is available if the plane does not belong to the body.

     ·     Unfix - Defines a plane in model space. The command is available if the plane does not belong to the body.

     ·     ShowInDocument - focuses the plane in the center of the model space. The command is available when the plane is displayed.

     ·     Rebuild - rebuilds the object in model space.

Add work axis

CAD drafting 3D Module 1266Main menu: 3D - 3D Features - CAD software 3D Module 1267Add work axis.

CAD drawing 3D Module 1268Ribbon: 3D Tools - Solid Editing - CAD drafting 3D Module 1269Add work axis.

CAD software 3D Module 1270Toolbar: 3D - CAD drawing 3D Module 1271Add work axis.

CAD drafting 3D Module 1272Command line: ADDWA.

A tool that allows you to add a new axis to the model space.

Procedure

1. Call command CAD software 3D Module 1273"Add work axis".

2. Choose how to draw an axis from the context menu or command line:

     ·     select object - the construction of the plane by the choice of the edge of the part.

     ·     2PT - plane construction by two points.

     ·     AXIS - the construction of an axis along a segment: edges, axes of symmetry, free geometry.

     ·     2PLN - the construction of an axis on the line of intersection of two planes.

     ·     WA_NORM2CURV - the construction of the axis is normal to the curve. To build, you must specify a curve and a point.

     ·     WA_NORM2SURF - the construction of an axis normal to the surface. To build, you must specify a surface and a point.

3. Select the required objects according to the selected axis construction method. To facilitate the selection of "the main coordinate system selection items", commands will be available in the context menu:

     ·     Origin - Selects the point of intersection of the principal axes of coordinates.

     ·     X, Y, Z - Selects axes of the main coordinate system.

     ·     XY, YZ, ZX - Selects the planes of the main coordinate system.

4. The "Work axis" object will be created and added to "3D History".

Properties

Does not have individual properties.

Grips

CAD drawing 3D Module 1274Moving grip - serves to move the axis in the model space. If the axis belongs to the body, it moves with it.

3D History

 CAD drafting 3D Module 1275Work axis. It can be located in the root of the tree and be part of objects  CAD software 3D Module 1276"Part".

The following shortcut menu commands are available:

     ·     Rename (F2) - allows you to rename an axis.

     ·     Delete (Del) - removes the axis and related objects from the tree and model space.

     ·     Hide - hides the axis map in model space.

     ·     Show - shows the display of the axis in model space.

     ·     Fix - fixes the axis in the model space. An anchor label is added to the axis icon. The command is available if the axis does not belong to the body.

     ·     Unfix - Defines an axis in model space. The command is available if the axis does not belong to the body.

     ·     ShowInDocument - focuses the axis in the center of the model space. The command is available when the axis is displayed.

     ·     Rebuild - rebuilds the object in model space.

Add work point

CAD drawing 3D Module 1277Main menu: 3D - 3D Features - CAD drafting 3D Module 1278Add work point.

CAD software 3D Module 1279Ribbon: 3D Tools - Solid Editing - CAD drawing 3D Module 1280Add work point.

CAD drafting 3D Module 1281Toolbar: 3D - CAD software 3D Module 1282Add work point.

CAD drawing 3D Module 1283Command line: ADDWPT.

A tool that allows you to add a new point to the model space.

Procedure

1. Call command CAD drafting 3D Module 1284"Add work point".

2. Choose how to build a point from the context menu or command line:

     ·     select object - the construction of a working point by choosing a point of the part.

     ·     VERTEX - the construction of a point along the existing working point, the vertex of the body, the middle of the part's rib, the characteristic points of free geometry, and so on.

     ·     CENTER - construction of the point at the central point of the element.

     ·     2CRV - the construction of a point at the intersection of two curves.

     ·     CRVSURF - the construction of a point in the intersection of a curve and a surface.

     ·     3PLN - the construction of a point in the intersection of three planes.

3. Select the required objects according to the selected way of constructing the point. To facilitate the selection of the "main coordinate system selection items", the following commands will be available in the context menu:

     ·     Origin - Selects the point of intersection of the principal axes of coordinates.

     ·     X, Y, Z - Selects axes of the main coordinate system.

     ·     XY, YZ, ZX - Selects the planes of the main coordinate system.

4. The "Work point" object will be created and added to "3D History".

Properties

Does not have individual properties.

Grips

CAD software 3D Module 1285Moving grip - serves to move a point in the model space. If the point belongs to the part, it moves with it.

3D History

 CAD drawing 3D Module 1286Work point. Can be located in the root of the tree and enter the structure of objects CAD drafting 3D Module 1287"Part".

The following shortcut menu commands are available:

     ·     Rename (F2) - allows you to rename a point.

     ·     Delete (Del) - removes a point and related objects from the tree and model space.

     ·     Hide - hides the display of a point in the model space.

     ·     Show - shows the display of a point in the model space.

     ·     Fix - fixes a point in the model space. An anchor label is added to the point icon. The command is available if the point does not belong to the part.

     ·     Unfix - defixes a point in model space. The command is available if the point does not belong to the part.

     ·     ShowInDocument - focuses the point in the center of the model space. The command is available when the point is displayed.

     ·     Rebuild - rebuilds an object in model space.

3D Constraint

Mate 3D Constraint

Important!

To use this functionality, the 3D modeling engine C3D is required.

CAD software 3D Module 1288Main menu:  3D - 3D Features - CAD drawing 3D Module 1289Mate 3D Constraint.

CAD drafting 3D Module 1290Ribbon: 3D Tools - 3D Constraint - CAD software 3D Module 1291Mate 3D Constraint.

CAD drawing 3D Module 1292Toolbar: 3D - CAD drafting 3D Module 1293Mate 3D Constraint.

CAD software 3D Module 1294Command line: 3DMATE.

The command allows you to impose a 3D constraint "Mate" on objects.

Procedure

1. Call command CAD drawing 3D Module 1295"Mate 3D Constraint";

Important!

When applying a constraint, at least one solid must be unfixed.

2. Select the geometry of the first solid (plane, edge, or point);

CAD drafting 3D Module 1296

3. Select the geometry of the second solid (plane, edge, or point);

CAD software 3D Module 1297

Note:

Alignment is performed along the normals of the selected geometry. When you select a plane, the normal is perpendicular to the plane. When you select an edge, the normal is along the edge. When you select a point, the normal is along the Z axis.

4. Enter the distance between the first or second geometry or select the "Flush" context menu command (for planes only);

CAD drawing 3D Module 1298

5. Constraint is applied, and CAD drafting 3D Module 1299"Mate constraint" objects are added to the "3D History" for each participating solid.

Edit

CAD software 3D Module 1300"Mate constraint". As part of the CAD drawing 3D Module 1301body.

The following context menu commands are available:

     ·     Edit - causes constraint to be edited.

     ·     End edit - completes the previously started editing.

     ·     Rename (F2) - allows you to rename the constraint.

     ·     Delete (Del) - delete constraint.

Insert 3D Constraint

Important!

To use this functionality, the 3D modeling engine C3D is required.

CAD drafting 3D Module 1302Main menu:  3D - 3D Features - CAD software 3D Module 1303Insert 3D Constraint.

CAD drawing 3D Module 1304Ribbon: 3D Tools - 3D Constraint - CAD drafting 3D Module 1305Insert 3D Constraint.

CAD software 3D Module 1306Toolbar: 3D - CAD drawing 3D Module 1307Insert 3D Constraint.

CAD drafting 3D Module 1308Command line: 3DINSERT.

The command allows you to impose a 3D constraint "Insert" on objects.

Procedure

1. Call command CAD software 3D Module 1309"Insert 3D Constraint";

Important!

When applying a constraint, at least one body must be unfixed.

2. Select the edge of the first body (circle, arc);

CAD drawing 3D Module 1310

Important!

A spline can be mistaken for a circle. Such a situation may arise, for example, when the edge of the hole is on a curved (cylindrical) plane.

3. Select the edge of the second body (circle, arc);

CAD drafting 3D Module 1311

Important!

A spline can be mistaken for a circle. Such a situation may arise, for example, when the edge of the hole is on a curved (cylindrical) plane.

4. Enter the distance between the first or second geometry or select the "Co-Directional" context menu command;

CAD software 3D Module 1312

5. Constraint is applied, and CAD drawing 3D Module 1313"Insert constraint" objects are added to the "3D History" for each participating solid.

Edit

CAD drafting 3D Module 1314"Insert constraint". As part of the CAD software 3D Module 1315body.

The following context menu commands are available:

     ·     Edit - causes constraint to be edited.

     ·     End edit - completes the previously started editing.

     ·     Rename (F2) - allows you to rename the constraint.

     ·     Delete (Del) - delete constraint.

Angle 3D Constraint

Important!

To use this functionality, the 3D modeling engine C3D is required.

CAD drawing 3D Module 1316Main menu:  3D - 3D Features - CAD drafting 3D Module 1317Angle 3D Constraint.

CAD software 3D Module 1318Ribbon: 3D Tools - 3D Constraint - CAD drawing 3D Module 1319Angle 3D Constraint.

CAD drafting 3D Module 1320Toolbar: 3D - CAD software 3D Module 1321Angle 3D Constraint.

CAD drawing 3D Module 1322Command line: 3DANGLE.

The command allows you to impose a 3D constraint "Angle" on objects.

Procedure

1. Call command CAD drafting 3D Module 1323"Angle 3D Constraint";

Important!

When applying a constraint, at least one body must be unfixed.

2. Select the geometry of the first body (plane or edge);

CAD software 3D Module 1324

3. Select the geometry of the second body (plane or edge);

CAD drawing 3D Module 1325

4. Select "Axis of rotation" if necessary. When specifying an angle between two primitives, the default angle scheme is used in the range 0-180. In order to cover the entire range of angles, an axis of rotation is needed. Also, setting the axis allows you to more correctly determine the direction of rotation. The axis must be perpendicular to both directions;

5. Enter the angle in degrees between the first or second geometry;

CAD drafting 3D Module 1326

6. Constraint is applied, and CAD software 3D Module 1327"Angle constraint" objects are added to the "3D History" for each participating solid.

Edit

CAD drawing 3D Module 1328"Angle constraint". As part of the CAD drafting 3D Module 1329body.

The following context menu commands are available:

     ·     Edit - causes constraint to be edited.

     ·     End edit - completes the previously started editing.

     ·     Rename (F2) - allows you to rename the constraint.

     ·     Delete (Del) - delete constraint.

Tangent 3D Constraint

Important!

This functionality requires a C3D 3D modeling engine.

CAD software 3D Module 1330Main menu:  3D - 3D Features - CAD drawing 3D Module 1331Tangent 3D Constraint.

CAD drafting 3D Module 1332Ribbon: 3D Tools - 3D Constraint - CAD software 3D Module 1333Tangent 3D Constraint.

CAD drawing 3D Module 1334Toolbar: 3D - CAD drafting 3D Module 1335Tangent 3D Constraint.

CAD software 3D Module 1336Command line: 3DTANGENT.

The command allows you to impose a 3D constraint "Tangent" on objects.

The Tangent 3D constraint allows you to create more complex surface tangencies than the Mate 3D constraint.

Constraint is superimposed on:

• cylinder to plane;

• cylinder to cylinder;

• cone to plane;

• sphere to cylinder;

• sphere to plane;

• circular edge to straight edge;

• circular edge to circular edge.

Procedure

1. Call command CAD drawing 3D Module 1337"Tangent 3D Constraint";

Important!

When applying a constraint, at least one body must be unfixed.

2. Select the geometry of the first solid;

CAD drafting 3D Module 1338

3. Select the geometry of the second body;

CAD software 3D Module 1339

4. Constraint is applied, and CAD drawing 3D Module 1340"Tangent constraint" objects are added to the "3D History" for each participating solid.

CAD drafting 3D Module 1341

Edit

CAD software 3D Module 1342"Tangent constraint". As part of the CAD drawing 3D Module 1343 body.

The following context menu commands are available:

     ·     Edit - causes constraint to be edited.

     ·     End edit - completes the previously started editing.

     ·     Rename (F2) - allows you to rename the constraint.

     ·     Delete (Del) - delete constraint.

Symmetry 3D Constraint

Important!

This functionality requires a C3D 3D modeling engine.

CAD drafting 3D Module 1344Main menu:  3D - 3D Features - CAD software 3D Module 1345Symmetry 3D Constraint.

CAD drawing 3D Module 1346Ribbon: 3D Tools - 3D Constraint - CAD drafting 3D Module 1347Symmetry 3D Constraint.

CAD software 3D Module 1348Toolbar: 3D - CAD drawing 3D Module 1349Symmetry 3D Constraint.

CAD drafting 3D Module 1350Command line: 3DSYMMETRY.

The command allows you to impose a 3D constraint "Symmetry" on objects.

The Symmetry 3D constraint allows you to align 3D solid elements symmetrically about a selected plane.

Procedure

1. Prepare objects: two symmetry objects and a plane. A face of a solid can be used as a plane.

CAD software 3D Module 1351

2. Call command CAD drawing 3D Module 1352"Symmetry 3D Constraint".

Important!

When applying a constraint, at least one body must be unfixed.

3. Select the plane of the first solid.

CAD drafting 3D Module 1353

4. Select the plane of the second solid.

CAD software 3D Module 1354

5. Select the plane relative to which the objects will be symmetrically positioned.

CAD drawing 3D Module 1355

6. Constraint is applied, and CAD drafting 3D Module 1356"Symmetry constraint" objects are added to the "3D History" for each participating solid.

The distance from the first selected face to the plane will be the base for the second selected face.

CAD software 3D Module 1357

Edit

CAD drawing 3D Module 1358"Symmetry constraint". As part of the CAD drafting 3D Module 1359 body.

The following context menu commands are available:

     ·     Edit - causes constraint to be edited.

     ·     End edit - completes the previously started editing.

     ·     Rename (F2) - allows you to rename the constraint.

     ·     Delete (Del) - delete constraint.

Converts

Convert to Mesh

CAD software 3D Module 1360Main menu: 3D - CAD drawing 3D Module 1361Convert to Mesh.

CAD drafting 3D Module 1362Ribbon: 3D Tools - Transform - CAD software 3D Module 1363Convert to Mesh.

CAD drawing 3D Module 1364Toolbar: 3D - CAD drafting 3D Module 1365Convert to Mesh.

CAD software 3D Module 1366Command line: MESHSMOOTH.

The tool allows you to convert "Parametric solid" (3D) and "3D Solid" in the object "Polyface Mesh".

Procedure

1. Call command CAD drawing 3D Module 1367"Convert to Mesh";

2. Specify the objects that need to be converted;

CAD drafting 3D Module 1368

3. Press the key "Enter (Space)";

4. Objects will be converted.

CAD software 3D Module 1369

Note:

If the objects were selected before the command "Convert to Mesh" is called, the conversion will be performed automatically immediately after the command is called.

Convert to Solid

CAD drawing 3D Module 1370Main menu: 3D - CAD drafting 3D Module 1371Convert to Solid.

CAD software 3D Module 1372Ribbon: 3D Tools - Transform - CAD drawing 3D Module 1373Convert to Solid.

CAD drafting 3D Module 1374Toolbar: 3D - CAD software 3D Module 1375Convert to Solid.

CAD drawing 3D Module 1376Command line: CONVTOSOLID.

The tool allows you to convert an object "Polyface Mesh" in the object "3D Solid".

Procedure

1. Call command CAD drafting 3D Module 1377"Convert to Solid";

2. Specify the objects that need to be converted;

CAD software 3D Module 1378

3. Press the key "Enter (Space)";

4. Objects will be converted.

CAD drawing 3D Module 1379

Note:

If the objects were selected before the command "Convert to sloid"is called, the conversion will be performed automatically immediately after the command is called.

2D Views

Toolbar for creating flat views and cuts from a 3D model.

CAD drafting 3D Module 1380

By default, views are placed on the plane XoY.

Note:

It is recommended to place views in the main coordinate system in order to avoid possible problems with the display of annotations.

By default, global settings are used when inserting new views. Changes in global settings made after inserting a new view will be reflected in this view.

If you change any view parameter, this parameter will be unsettled from global settings and further changes of this parameter in global settings will not affect this view. 

To remove the parameter override, use the command  - Redefinition parameters.

Section Plane

CAD software 3D Module 1381Main menu: 3D - 2D Views - CAD drawing 3D Module 1382Section.

CAD drafting 3D Module 1383Ribbon: 3D Tools - Section - CAD software 3D Module 1384Section Plane.

CAD drawing 3D Module 1385Toolbar: 2D Views - CAD drafting 3D Module 1386Section.

CAD software 3D Module 1387Command line: VIEWSECTION.

The team is designed to get a flat section of the body.

Procedure

1. Call command CAD drawing 3D Module 1388"Section Plane".

2. Select the cutting plane:

     ·     The secant plane can be any plane (working, plane GCS),as well as a flat surface of the solid.

CAD drafting 3D Module 1389CAD software 3D Module 1390

     ·     A plane section can also be obtained by dissecting the solid not by a plane, but by a line. To do this, you must specify two points that will indicate the direction of the plane. If the cutting plane is indicated by a line, the plane will always be perpendicular to the XY plane.

CAD drawing 3D Module 1391CAD drafting 3D Module 1392

     ·     A flat section can be obtained by indicating three points. To do this, select the command "3Points" from the context menu and select 3 points.

CAD software 3D Module 1393CAD drawing 3D Module 1394

3. Specify the sheet where the view will be located. The command will offer a choice of all the sheets and model space that are in the document.

4. Select the position of the main planar section view. The view on the sheet is scaled so that it enters the sheet space and still has room for auxiliary projections.

CAD drafting 3D Module 1395

5. Insert projected section views. Press the "Enter" key to finish inserting projection views. Auxiliary projections are inserted on the same sheet where the main view is inserted.

CAD software 3D Module 1396

6. Will be built "NcDbSection" and "DriwingViewBlock". The corresponding objects will be added to the "3D History".

Properties

The following object "NcDbSection" properties are available in the properties panel:

     ·     Is Live - controls the display of a section on a three-dimensional model. Parts, through which the cutting plane passes, will receive an incision.

Note:

The cut on the 3D model is for viewing only. On such planes it is impossible to build sketches and the rest of the geometry.

 

No

Yes

CAD drawing 3D Module 1397

CAD drafting 3D Module 1398

 

     ·     Name - Name section. It is recommended to change the name in "3D History".

     ·     Type - type section:

Plane - section on 1 plane

CAD software 3D Module 1399

Boundary - section along 4 planes

CAD drawing 3D Module 1400

Volume - section along 6 planes

CAD drafting 3D Module 1401

Grips

CAD software 3D Module 1402

CAD drawing 3D Module 1403 - grips change the position of the section in space. The upper grip is responsible for the movement, the lower grip is for the slope;

CAD drafting 3D Module 1404 - grips changes the position of the cutting plane (grip allows you to change the position of the plane only in one axis), the number of grips corresponds to the number of secant planes;

CAD software 3D Module 1405 - grip shear direction changes;

CAD drawing 3D Module 1406 - grip change of secant plane properties: Section Plane, Section Boundary, Section Volume.

3D History

CAD drafting 3D Module 1407 Section. In "3D History" section is located in the root folder CAD software 3D Module 1408"Sections" and has child objects CAD drawing 3D Module 1409"View".

The following shortcut menu commands are available:

     ·     Rename (F2) - rename a section.

     ·     Delete (Del) - deletes the section and child objects from the model tree and model space.

     ·     Hide - hides the section and child objects from the model space. Section icon becomes inactive.

     ·     Show - shows the section and child objects in the model space. Section icon becomes active.

     ·     ShowInDocument - focuses and highlights the section at the center of the model space.

     ·     Rebuild - rebuilds an object in model space.

2D View

CAD drafting 3D Module 1410Main menu: 3D - 2D Views - CAD software 3D Module 1411Projected view.

CAD drawing 3D Module 1412Ribbon: 3D Tools - Section - CAD drafting 3D Module 14132D View.

CAD software 3D Module 1414Toolbar: 2D Views - CAD drawing 3D Module 1415Projected view.

CAD drafting 3D Module 1416Command line: DRAWINGVIEW.

The command allows you to create two-dimensional views from the three-dimensional part.

Procedure

1. Call command CAD software 3D Module 1417"2D View".

2. Select the parts you want to create from. To complete the selection, press the "Enter" key.

CAD drawing 3D Module 1418

3. Specify the sheet where the view will be located. The command will offer a choice of all the sheets and model space that are in the document.

4. Position the main view on the plane. The view on the sheet is scaled so that it enters the sheet space and still has room for auxiliary projections.

CAD drafting 3D Module 1419

5. Position the necessary auxiliary projection views: flat and isometric. To finish inserting views, press the "Enter" key. Auxiliary projections are inserted on the same sheet where the main view is inserted.

CAD software 3D Module 1420

6. Will be created "Projected Views" and added to "3D History".

Edit

The 2D View is called for editing: by the "Edit" command of the context menu on the view, by the "Edit" command from the history of 3D constructions, by double-clicking the LMB.

Editing is allowed if the view does not depend on the section object.

If the view is in paper space, it switches to model space.

In edit mode, all currently projected objects are selected, you can add objects by selecting a new object, or remove them by deselecting an object.

To complete editing, you must press the "Enter" key, all related views will be rebuilt according to a new set of objects.

Properties

The following object properties are available in the properties panel:

Name - Name of the view. The name of the view is recommended to be changed in the "3D History".

Fill Angle - Angle of rotation.

Enable Update - The parameter controls the automatic view update when the part geometry is changed.

Alignment - The parameter controls alignment by coordinates with the set step when moving the view.

Show Hidden Lines - The parameter controls the display of hidden lines.

Show hatch - The parameter controls the display of hatching.

Grips

CAD drawing 3D Module 1421Moving grip - serves to move the view in model space.

3D History

CAD drafting 3D Module 1422 View. In the "3D History" View belongs to part or section.

The following shortcut menu commands are available:

     ·     Rename (F2) - allows you to rename a view.

     ·     Delete (Del) - removes the view from the tree and model space.

     ·     Hide - hides the view from the model space. View icon becomes inactive.

     ·     Show - shows the view in the model space. View icon becomes active.

     ·     Show hidden lines - shows hidden lines.

     ·     Hide hidden lines - hide hidden lines.

     ·     ShowInDocument - focuses and highlights the view in the center of the model space.

     ·     Rebuild - rebuilds an object in model space.

2D Projection

CAD software 3D Module 1423Main menu: 3D - 2D Views - CAD drawing 3D Module 14242D Projected View.

CAD drafting 3D Module 1425Ribbon: 3D Tools - Section - CAD software 3D Module 14262D Projection.

CAD drawing 3D Module 1427Toolbar: 2D Views - CAD drafting 3D Module 14282D Projected View.

CAD software 3D Module 1429Command line: PROJECTIONVIEW.

The command creates a projection for the created views.

Procedure

1. Call command CAD drawing 3D Module 1430"2D Projection".

2. Select the previously created view.

CAD drafting 3D Module 1431

3. Position the projections on the plane. To complete the insertion, press the "Enter" key. Projection views vary depending on the location relative to the selected species.

CAD software 3D Module 1432

4. Will be created new objects Projected View" and added to "3D History".

CAD drawing 3D Module 1433

2D Section

CAD drafting 3D Module 1434Main menu: 3D - 2D Views - CAD software 3D Module 14352D Section View.

CAD drawing 3D Module 1436Ribbon: 3D Tools - Section - CAD drafting 3D Module 14372D Section.

CAD software 3D Module 1438Toolbar: 2D Views - CAD drawing 3D Module 14392D Section View.

CAD drafting 3D Module 1440Command line: SECTIONVIEW.

The command creates a 2D section view of the created projected views.

Procedure

1. Select Projected View. The command will draw sections in the same place as the main view. The scale is taken from the main view.

CAD software 3D Module 1441

2. Call command CAD drawing 3D Module 1442"2D Section".

3. Specify the first and second cut points.

CAD drafting 3D Module 1443

4. Place the view on the plane. Depending on the location (left or right of the line), the direction of the view will change.

CAD software 3D Module 1444

5. Will be created new object  "Projected View" and added to "3D History".

Hatching Sections

CAD drawing 3D Module 1445Main menu: 3D - 2D Views - CAD drafting 3D Module 1446Hatching Sections.

CAD software 3D Module 1447Ribbon: 3D Tools - 2D Views - CAD drawing 3D Module 1448Hatching Sections.

CAD drafting 3D Module 1449Toolbar: 2D Views - CAD software 3D Module 1450Hatching Sections.

CAD drawing 3D Module 1451Command line: DRAWINGVIEWAUTOHATCH.

The command analyzes all cuts in the drawing and corrects them so that each of the parts in all cuts has the same pitch and angle of dashed lines, which is different from other parts.

Procedure

1. Previously, a section with a 2D view must be created, containing several parts.

CAD drafting 3D Module 1452

2. Call command CAD software 3D Module 1453"Hatching Sections". The team will analyze and correct the hatches. After the adjustment, the command will automatically end.

Before

CAD drawing 3D Module 1454

After

CAD drafting 3D Module 1455

 

 

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